Contents

1. TURN TOOLBAR. 4

1.1 REVOLVE. 4

1.1.1 Sketch Entity Tool Bar. 5

1.1.1.a  Line Segment 6

1.1.1.b  Arc. 6

1.1.1.c   Inverted Arc. 8

1.1.1.d  3 Point Arc. 9

1.2 SUBSECTION.. 10

1.3 GROOVE. 12

1.3.1 Trapezoidal Groove. 14

1.3.2     Rectangular Groove. 15

1.3.3     Filleted Trapezoidal Groove. 17

1.3.4     Filleted Rectangular Groove. 18

1.4 STEP. 20

1.5 FILLET. 22

1.6 CHAMFER. 23

1.6.1     L1 X L2 Chamfer. 24

1.6.3     L1 X q Chamfer. 25

1.6.3     CL X q Chamfer. 26

1.7 HOLE. 27

1.7.1 Penetration type. 28

1.7.2 Hole type. 29

1.7.2.a Hole. 30

1.7.2.b Tapered Hole. 30

1.7.2.c Counter Sink Hole. 31

1.7.2.d Counter Bore Hole. 32

1.7.2.e Counter Drill Hole. 33

1.7.3 Hole Pattern and No of Holes. 34

1.7.3 Hole Orientation. 35

1.7.3 Bottom type. 37

1.7.4 Threaded. 38

1.8 THREAD.. 38

1.9 DELETE. 40

2.    Side Toolbar Features. 41

2.1 Horizontal Constraint ON/OFF. 41

2.2 Vertical Constraint ON/OFF. 42

2.3 Grid Snap ON/OFF. 43

2.4 Dimensions ON/OFF. 43

2.5 Redundant Dimensions ON/OFF. 44

2.6 3D Preview ON/OFF. 45

2.7 Transparency ON/OFF. 46

2.8 Auto adjust profile ON/OFF. 47

2.9 Open Mouse Help panel 49

2.10 Zoom In. 50

2.11 Zoom Out 50

2.12 Zoom All 51

2.13 Zoom Window.. 51

2.14 Move (Pan) 52

2.15 Rotate. 53

2.16 Grid ON/OFF. 53

3. Plane Section Toolbar. 54

3.1 XY - Plane. 55

3.2 YZ - Plane. 56

3.3 ZX - Plane. 57

3.4 Face – Plane. 58

3.5 Invert – Plane. 60

4. Page Side Toolbar. 62

5. File Module Toolbar. 62

5.1 New.. 62

5.2 Open. 63

5.3 Save. 63

5.4 Save As. 64

5.4.1 Save As STL. 64

5.4.2 Save As STL (Binary) 65

5.4.3 Save As OBJ 65

5.4.4 Save As GLTF. 66

5.4.5 Save As GLB. 66

5.4.6 Save As STEP. 66

6. View Module Toolbar. 67

6.1 Undo. 67

6.2 Redo. 67

6.3 Clear. 68

6.4 Views. 68

7. Settings and Help Toolbar. 73

7.2 Settings. 73

7.2.1 Grid Settings. 74

7.2.2 Theme Settings. 74

7.2.3 Save As Settings. 77

7.2.4 Arrow dimensions Settings. 78

7.2.5 Turn module Settings. 78

7.2.5.a Groove Settings. 79

7.2.5.b Fillet Settings. 82

7.2.5.c Chamfer Settings. 82

7.2.5.d Hole Settings. 84

7.2.5.e Step Settings. 87

7.3 Help. 87

7.3.1 Help. 88

7.3.2 Tutorial Videos. 88

7.3.3 About 88

8. Special features. 88

8.1 Rotator. 88

8.2 Feature Tree. 89

8.3 Contextual Help. 89

9. Alarvy File Format 91

9.1. Parts. 92

9.1.1 Profile. 94

9.1.2 Features. 95

9.1.3 Hole Features. 96

9.1.4 Threads. 97

9.1.5 Dimension Positions. 97

 

1. TURN TOOLBAR

 

Fig 1.1 Turn Toolbar

ALARVY Turn module contains multiple features specifically to create 3D CAD models of turned parts or revolved parts or parts that can be manufactured in lathes and turning centres.

ALARVY Turn module comes with the following features

 

                                 I.            Revolve

                               II.            Subsection

                             III.            Groove

                            IV.            Step

                              V.            Fillet

                            VI.            Chamfer

                           VII.            Hole

                         VIII.            Thread

 

1.1 REVOLVE

Fig 1.1.1 Revolve button

 

       On clicking the Revolve button, it automatically shows the Top view.

       It already has an axis and no need to draw an axis like other modelers.

       It requires only half sketch so that it can revolve the sketch about 360 degrees.

       The sketch can contain lines and arcs.

       It allows only a closed sketch to be created and hence the sketch uses the last point of the first entity as the start point of the next entity.

       There is no separate sketcher and 3D model view in AlarvyCAD. Both are integrated.

       By default, Grid, Horizontal Constraint, Vertical Constraint, Grid Snap are ON.

       On clicking Revolve, after clicking the first point, sketch entity tool bar appears in the right to choose line or arc or inverted arc or 3 point arc or to close the sketch. Note that line option is on by default. Refer Fig 1.1.2 and Section 1.1.1

       The sketch requires a minimum of 3 points or 2 entities (lines/arcs) to close the Sketch.

       Keyboard shortcuts for various buttons are given in brackets: Line (L), Arc (A), Invert (I / down arrow), 3 Point (3) and Close (C / Esc).

       On every click of a point in the Sketch, Diameter and Length dimensions will automatically appear for each point.

 

1.1.1 Sketch Entity Tool Bar

Fig 1.1.2 Sketch entity tool bar

 

  • On clicking the Revolve or Subsection button, sketcher mode is turned On.
  • In Sketcher mode, only 2d sketch is shown in top view.
  • After adding first point to the sketch, Entity toolbar appears in the right, next to side toolbar.
  • This allows the user to select a Line segment or Arc or Inverted arc or 3-Point Arc to be drawn to the next point of the sketch.

 

1.1.1.a  Line Segment

 

·       Adds a line from the previous added point to the current mouse position.

·       Refer Fig 1.1.3

Fig 1.1.3 Line segment

 

1.1.1.b  Arc

 

·       Adds an arc from the previous added point to the current mouse position.

·       It is initially drawn such that the first point is tangential to the previous entity (lines/arc). In other words, tangent continuity is maintained initially. Refer Fig 1.1.4 and 1.1.5.

·       On editing the arc dimensions, the tangent continuity may not get maintained depending on the dimensions.

·       For an arc, the dimensions shown in black in the Fig 1.1.6 defines the arc: start diameter, end diameter, arc radius and length between the first and last point of the arc.

Fig 1.1.4 Arcs while sketching maintaining tangential continuity

 

Fig 1.1.5 Arcs while sketching not maintaining tangential continuity

 

Fig 1.1.6 Arcs after sketching

 

1.1.1.c   Inverted Arc

 

       Inverted arc is initially drawn such that the first point is not tangential to the previous entity (lines/arc) and is inverted with respect to a tangential arc.

       Refer Fig 1.1.7 and 1.1.8.

Fig 1.1.7 Creation of inverted arc

 

Fig 1.1.8 Creation of inverted arc

 

1.1.1.d  3 Point Arc

 

       A 3 Point Arc is defined by 3 points through which the arc passes. In Fig 1.1.9, the first point of a 3 Point Arc is the last point of the previous line and the second point is shown as the end point of a dashed line.

       On clicking the third point, the arc appears as shown in the Fig 1.1.10.

       For a 3 Point Arc, the dimensions shown in black in Fig 1.1.11 defines the arc: start diameter, end diameter, arc radius and length between the first and last point of the arc.

Fig 1.1.9 Creation of three point arc

 

Fig 1.1.10 Creation of three point arc

 

Fig 1.1.11 Three point arc

 

1.2 SUBSECTION

 

Fig 1.2.1 Subsection

 

·       Click on Subsection once a model is created.

·       UI enters Sketcher mode.

·       Create subsection points like Revolve model.

·       First and last points of a subsection sketch should intersect with a model indicating the start and end of a subsection.

·       Lines, arcs or 3 Point arcs are supported in Subsection.

·       For Undo of Subsection, after undo, press Esc to exit Sketcher mode.

 

Subsection Sketcher mode:

·       A 3D Model can be edited in sketcher mode.

·       In sketcher mode, model is shown as a 2d sketch.

·       Red point is seen on mouse move. It turns blue when it is over any edge of the model.

·       On mouse click, first point of subsection is added to the sketch along with dimensions.

·       Second point of subsection cannot be on the same edge of the model.

·       On mouse move, a line segment is shown starting from previously added point.

·       There is an entity tool bar next to side toolbar in right which has an option to choose Line, Arc, Inverted arc or 3 point arc. Line is default option.

·       Based on selected option, same is drawn from previously added point of the sketch to the current mouse position.

·       With subsequent clicks, others points are added to the sketch with corresponding dimensions.

·       Last point of subsection should be on the revolve sketch edge to form a closed sketch.

·       Once a closed sketch is created, it exits sketcher mode and 3D Model is shown.

 

Fig 1.2.2 Subsection creation – in sketch mode

 

Fig 1.2.3 Subsection - after creation

 

1.3 GROOVE

 

Fig 1.3.1 Groove in toolbar

 

 

·       Click on Groove to select the type of groove to be inserted in model.

·       Four different types of grooves are available

                                 i.            Trapezoidal

                               ii.            Rectangular

                             iii.            Filleted Trapezoidal

                             iv.            Filleted Rectangular

·       These types have fixed dimensions while insertion. However, dimensions can be edited after inserting.

 

Insertion:

·       Select a groove type to insert in model.

·       Shows the groove in red until an edge in the model is selected to insert groove. Refer Fig 1.3.2

·       Groove turns blue once an edge in model is selected. Refer Fig 1.3.3

·       Click on the edge to insert.

Fig 1.3.2 Groove on mouse move before insertion

 

Fig 1.3.3 Groove on edge on mouse move before insertion

 

1.3.1 Trapezoidal Groove

 

Fig 1.3.4 Trapezoidal groove

 

·       Inserts a Trapezoidal shaped groove in the edge of the model. Refer Fig 1.3.5

·       Select Groove à Trapezoidal.

·       Select an edge in the model to insert.

·       It has fixed dimension while insertion. These dimensions are specified in Settings àTurn module settings à Trapezoidal Groove.

·       Dimensions can be edited after insertion.

 

Fig 1.3.5 Trapezoidal groove while insertion

 

Fig 1.3.6 Trapezoidal groove after insertion – 3D view

 

1.3.2     Rectangular Groove

 

Fig 1.3.7 Rectangular groove

 

·       Inserts a Rectangular shaped groove in the highlighted edge of the model. Refer Fig 1.3.7

·       Select Groove à Rectangular.

·       Select an edge in the model to insert.

·       It has fixed dimension while insertion. These dimensions are specified in Settings àTurn module settings à Rectangular Groove.

·       Dimensions can be edited after insertion.

 

Fig 1.3.8 Rectangular groove while insertion

 

Fig 1.3.9 Rectangular groove after insertion – 3D view

 

1.3.3     Filleted Trapezoidal Groove

 

Fig 1.3.10 Filleted trapezoidal groove

 

·       Inserts a Trapezoidal shaped groove with filleted ends in the highlighted edge of the model. Refer Fig 1.3.9

·       Select Groove à Filleted Trapezoidal.

·       Select an edge in the model to insert.

·       It has fixed dimension while insertion. These dimensions are specified in Settings àTurn module settings à Filleted Trapezoidal Groove.

·       Dimensions can be edited after insertion.

 

Fig 1.3.11 Filleted trapezoidal groove while insertion

 

Fig 1.3.12 Filleted trapezoidal groove after insertion – 3D view

 

1.3.4     Filleted Rectangular Groove

 

Fig 1.3.13 Filleted Rectangular groove

 

·       Inserts a Rectangular shaped groove with filleted ends in the highlighted edge of the model. Refer Fig 1.3.11

·       Select Groove à Filleted Rectangular.

·       Select an edge in the model to insert.

·       It has fixed dimension while insertion. These dimensions are specified in Settings àTurn module settings à Filleted Rectangular Groove.

·       Dimensions can be edited after insertion.

 

Fig 1.3.14 Filleted rectangular groove while insertion

 

Fig 1.3.15 Filleted rectangular groove after insertion – 3D view

 

1.4 STEP

 

Fig 1.4.1 Step

 

·       Step feature inserts a step in model.

·       It has a slanting edge, base edge with a default angle between them.

·       It has fixed dimension while insertion. These dimensions are specified in Settings àTurn module settings à Step.

·       However, dimensions can be edited after inserting also.

 

Insertion:

 

·       On Click of Step, a step feature is shown in red on mouse move. Refer Fig 1.4.2

·       Feature turns blue once an edge in model is selected.

·       Click on the edge in model to insert the step.

·       Once the top edge of step is fixed on the model, base edge of the step automatically extends to reach the nearest right edge in the model and a step is created as shown in Fig 1.4.3.

 

Fig 1.4.2 Step before insertion

 

Fig 1.4.3 Step created

 

1.5 FILLET

 

Fig 1.5.1 Fillet

 

·       Adds roundness to the curved edges.

·       On mouse hover, curved edge of the model is highlighted in yellow.

·       Click on that edge or point to add fillet.

·       When 3D preview is OFF, fillet can be created by selecting a vertex in the revolve sketch.

·       Fillets have one dimension (Radius), which is editable.

·       To edit the dimension, Click on Dimension R near the fillet and type updated value.

·       Fillet Radius can also be edited by dragging the FilletCenter highlighted in yellow in Fig 1.5.3

 

Fig 1.5.2 Fillet added

 

Fig 1.5.3 Fillet dimension edit by drag

 

1.6 CHAMFER

 

Fig 1.6.1 Chamfer

 

·       Chamfer inserts a slanting edge on the selected edge of the model.

·       Three types of chamfer are provided

                                i.            L1 X L2

                               ii.            L1 X q

                             iii.            CL X q

·       It has fixed dimension while adding. However, dimensions can be edited after inserting.

·       Edit Leader Dimension box has dimension params and chamfer type for editing. Refer Fig 1.6.4

·       Click on ü after editing in the editbar.

 

1.6.1     L1 X L2 Chamfer

 

·       Click on Chamfer à L1 X L2, to add this chamfer type.

·       When the edge or point is selected to add this chamfer type, a slanting edge is added as shown above.

·       L1 is the length from the point P in model and point of intersection with edge 1.

·       L2 is the length from the point P in model and point of intersection with edge 2.

·       Once the chamfer is added, dimensions L1 and L2 can be edited by clicking on them as in Fig 1.6.4

 

Fig 1.6.2 L1 X L2 Chamfer

 

Fig 1.6.3 L1 X L2 Chamfer added

 

Fig 1.6.4 Editing dimensions in chamfer

 

1.6.3     L1 X q Chamfer

 

Fig 1.6.5 L1 X q Chamfer

 

·       Click on Chamfer à L1 X q, to add this chamfer type.

·       When the edge or point is selected to add this chamfer type, a slanting edge is added as shown above.

·       L1 is the length from the point P in model and point of intersection with edge 1.

·       q is the angle between L1 and slant edge.

·       Once the chamfer is added, dimensions L1 and q can be edited by clicking on them as in Fig 1.6.6

 

Fig 1.6.6 L1 X q Chamfer

 

1.6.3     CL X q Chamfer

 

Fig 1.6.7 CL X q Chamfer

 

·       Click on Chamfer à CL X q, to add this chamfer type.

·       When the edge or point is selected to add this chamfer type, a slanting edge is added as shown above.

·       CL is the length of the slant edge in model added by Chamfer.

·       q is the angle between L1 and slant edge.

·       Once the chamfer is added, dimensions CL and q can be edited by clicking on them as in Fig 1.6.6

 

Fig 1.6.8 CL X q Chamfer

 

1.7 HOLE

 

Fig 1.7.1 Hole

 

·       Hole inserts hole feature in the model.

·       Create a model. Then Click Hole à Opens Hole settings panel.

·       Choose the hole attributes - penetration type, hole type, pattern, hole orientation, number of holes, bottom type and threaded option in the settings panel and click OK.

·       On mouse move, when cursor is outside the model or on the wrong face of the model, red coloured Circle appears. It turns blue when cursor is on right face.

·       On mouse click, hole is inserted with default dimensions. These dimensions are specified in Settings àTurn module settings à Hole.

·       It has fixed dimensions while insertion. However, dimensions can be edited after inserting.

·       Clicking hole leader dimensions opens Hole Attributes Editbar, which includes hole type, hole radius, penetration type, hole depth, Pitch Circle Diameter, angles based on hole type, etc. Refer Fig 1.7.2.

 

Hole Settings

1.7.1 Penetration type

 

·       Penetration specifies the hole penetration length into the model.

·       Penetration has two types –

1.      Blind

2.      Through

·       Blind – Blind type Hole has a fixed length penetration into the model from the point of click, Refer Fig 1.7.2.

·       This length dimension is editable after hole creation, Refer Fig 1.7.2.

·       Through – Through type Hole penetrates the whole model from the point of insertion to the opposite edge in model. Refer Fig 1.7.3.

·       Type of the Penetration can be changed even after hole is created by clicking on hole dimension and editing the Penetration type, Refer Fig 1.7.2.

 

Fig 1.7.2 Blind penetration type hole

 

Fig 1.7.3 Through penetration type hole

 

1.7.2 Hole type

 

·       Specifies the hole type

 

·       Different types of Hole are explained below

a)      Hole

b)      Tapered

c)      Counter Sink

d)      Counter Bore

e)      Counter Drill

 

1.7.2.a Hole 

 

o   Top and Bottom diameter of the hole remains same. Refer Fig 1.7.2, 1.7.3.

o   It has the following parameters – Diameter, Depth and PCD (Pitch Circle Diameter).

o   All dimensions can be edited by clicking the dimension after creation.

 

1.7.2.b Tapered Hole

 

o   Top and Bottom diameters are different. Appears tapered at one end. Refer Fig 1.7.4.

o   It has the following parameters – Top diameter, Bottom diameter, Cone angle, Hole depth and PCD.

o   All dimensions can be edited by clicking the dimension after hole creation.

 

Fig 1.7.4 Tapered hole

 

1.7.2.c Counter Sink Hole

 

o   It has a tapered head, cylindrical portion and a flat/conical end. Refer Fig 1.7.5.

o   It has the following parameters– Hole diameter, Hole depth, Counter Sink top diameter, Counter Sink cone angle, PCD.

o   All the dimensions can be edited by clicking the leader dimension after hole creation.

o   Follow dimension calculations shown in Fig 1.7.6.

o   Follow the contextual help at the bottom to know maximum and minimum values that can be set to the dimensions.

 

Fig 1.7.5 Counter sink hole

 

Fig 1.7.6 Dimensions of counter sink hole

 

1.7.2.d Counter Bore Hole

 

o   It has a counter bore head, a cylindrical portion and a flat/conical end. Refer Fig 1.7.6.

o   Counter bore head is defined by dimensions – Counterbore diameter and Counterbore height.

o   The cylindrical portion is defined by dimension - Hole diameter and PCD.

o   Hole depth is total length of the cylindrical portion and counter bore height.

o   All the dimensions can be edited by clicking the dimension after hole creation.

o   Follow dimension calculations shown in Fig 1.7.6.

o   Follow the contextual help at the bottom to know maximum and minimum values that can be set to the dimensions.

 

Fig 1.7.7 Counter bore hole

 

1.7.2.e Counter Drill Hole

 

o   It has a counter bore head followed by counter sink base, a cylindrical portion and a flat/conical end. Refer Fig 1.7.8.

o   Counter bore base is defined by dimensions – Counter bore diameter and Counter bore height.

o   Counter sink base is defined by dimensions – Counter sink top diameter and Cone angle.

o   Counter bore diameter and Counter sink top diameter are same and will always have same value.

o   The cylindrical part is defined by dimension - Hole diameter.

o   Counter Drill hole position is defined by PCD.

o   Hole Depth is total length of the cylindrical portion, counter sink portion and counter bore height.

o   All the dimensions can be edited by clicking the dimension after hole creation.

o   Follow the contextual help at the bottom to know maximum and minimum values that can be set to the dimensions.

 

Fig 1.7.8 Counter drill hole

 

1.7.3 Hole Pattern and No of Holes

 

·       Specifies the hole pattern – Single, Multiple, Circular Pattern types.

·       Single – Adds only one hole. So, number of holes is set to 1.

 

·       Multiple – Adds multiple number of holes as mentioned in number of holes tab. Holes are added one after another allowing the user to choose position. By default, 3 holes are added and the count is editable.

 

·       Circular Pattern – Adds multiple number of holes at one shot in circular pattern with just one click on the model. Refer Fig 1.7.9. By default, 5 holes are added but this number is editable in number of holes field.

 

Fig 1.7.9 Circular pattern hole

 

1.7.3 Hole Orientation

 

·       Specifies the hole Orientation – Axial, Radial, Vertical.

·       Axial – Hole is added to the model parallel to the Axis line. Before inserting, Hole will appear Red in colour if cursor is on cylindrical part of the model. It turns blue only over axial face. Refer Fig 1.7.10.

·       Radial – Hole is added to the model on the cylindrical part of the model. Axis of the hole is perpendicular to the Axis line. Before inserting, hole appears red in colour if cursor is on axial face of the model. It turns blue only over cylindrical face or conical face. Refer Fig 1.7.11.

·       Vertical – Hole is added vertically to the point of intersection on the model face. This hole cannot be added on axial face. Refer Fig 1.7.12.

 

Fig 1.7.10 Axial hole

 

Fig 1.7.11 Radial hole

 

Fig 1.7.12 Vertical hole

 

1.7.3 Bottom type

·       Specifies the bottom type of the hole – Flat or Conical.

·       Conical – Creates a hole with conical end at bottom. Ref Hole-1 in Fig 1.7.13.

·       Flat – Creates a hole with flat end at the bottom. Ref Hole-2 in Fig 1.7.13.

 

Fig 1.7.13 Conical and flat bottom hole

 

1.7.4 Threaded

·       Creates hole with or without threads based on the checkbox value.

·       Creates thread with ISO standard.

·       Threads are characterised by Diameter of the thread(M) and the Pitch.

·       These properties are editable in Hole Attributes Editbar, which can be opened on clicking hole dimensions.

·       Refer Fig 1.7.14 for hole with threads.

 

Fig 1.7.14 Threaded hole

 

 1.8 THREAD

 

Fig 1.8.1 Thread

 

·       This feature adds thread to the model.

·       Click Thread in Turn toolbar à Select an edge in the revolve sketch to draw threads.

·       Threads can be drawn on horizontal edges only.

·       Circular edge diameter at the left or right (as they are equal) is automatically taken as the thread diameter.

·       Created thread uses ISO Metric Profile standards.

·       If the diameter is not standard, closest matching diameter is selected for choosing the pitch.

·       AlarvyCAD automatically places an editable thread leader dimension which lists all the available pitches for the given diameter.

·       Available pitch values follow ISO Metric standard and the highest pitch is selected as default.

·       Dimensions includes the length for threaded area and clearance area.

·       Clearance dimension can be removed by making clearance dimension as zero.

·       AlarvyCAD Threads shown in Fig 1.8.2 are using virtual representation showing the helical structure. In reality, threads have grooves in them. Actual thread representations are avoided to make the profile lighter and rendering easier.

·       Internal threads can also be made by directly selecting the internal edge in sketch. Refer Fig 1.8.3.

 

Fig 1.8.2 External threads

 

Fig 1.8.3 Internal threads

 

1.9 DELETE

 

Fig 1.9.1 Delete

 

·       Select an entity from the feature tree and Click Delete in Turn toolbar.

·       This feature deletes that entity from the model.

·       Points, features like holes, grooves, subsections, fillets, etc can be removed.

·       To delete a point, Click on Delete button, select the point to be deleted from the sketch. Confirmation popup appears à Click Ok.

·       When a point is removed, line segment is added between previous and next points of the selected point and the sketch and 3D model are updated. Refer Fig 1.9.2, 1.9.3.

·       To delete a feature, choose that feature from feature tree and click on Delete button. Click Ok on confirmation popup.

Fig 1.9.2 Deleting the highlighted point in yellow

 

Fig 1.9.3 After deleting the selected point

 

2.    Side Toolbar Features

 

2.1 Horizontal Constraint ON/OFF

 

·       When Horizontal Constraint is ON, Sketcher forces the next point selection to be parallel to the Horizontal axis (X) of the sketch provided it is within a tolerance limit.

·       By default, Horizontal Constraint is ON.

 

Fig 2.1 Horizontal constraint ON/OFF button

 

2.2 Vertical Constraint ON/OFF

 

·       When Vertical Constraint is ON, Sketcher forces the next point selection to be parallel to the Vertical axis (Y) of the sketch provided it is within a tolerance limit.

·       By default, Vertical Constraint is ON. 

Fig 2.2 Vertical constraint ON/OFF button

 

2.3 Grid Snap ON/OFF

 

·       When Grid Snap is ON, Sketcher forces the next point selection to the nearest X or Y line segment of the Grid.

·       By default, Grid Snap is ON.

Fig 2.3 Grid snap ON/OFF button

 

2.4 Dimensions ON/OFF

 

·       Model Dimensions can be turned ON/OFF using this button.

·       By default, Dimensions is ON.

Fig 2.4 Dimensions ON/OFF button

 

Fig 2.5 Model with dimensions turned OFF

 

Fig 2.6 Model with dimensions turned ON

 

2.5 Redundant Dimensions ON/OFF

 

·       Redundant Dimensions in the Model can be turned ON/OFF using this button.

·       By default, Redundant Dimensions is ON to help editing the sketch easier, as each point in sketch has a diameter dimension and length dimension. The length dimension is not given, when two points are having same X coordinate value.

·       Refer Fig 2.8 for example.

Fig 2.7 Redundant dimensions ON/OFF button

 

Fig 2.8 Model with redundant dimension turned OFF

 

2.6 3D Preview ON/OFF

 

·       Switching 3D Preview ON, shows the solid 3D Model.

·       Switching 3D Preview OFF, hides the model and 2D sketch is shown.

·       By default, 3D Preview is ON.

Fig 2.9 3D preview ON/OFF button

 

Fig 2.10 Model with 3D sketch turned OFF

 

2.7 Transparency ON/OFF

 

·       Turning Transparency button ON, shows the transparent model which clearly depicts the inner and outer details of the model.

·       By default, Transparency is OFF.

Fig 2.11 Transparency ON/OFF button

 

Fig 2.12 Model with transparency ON

 

2.8 Auto adjust profile ON/OFF

 

·       With Auto adjust ON, Editing the dimensions moves the whole sketch right.

·       With Auto adjust OFF, editing the dimensions moves the immediate right points only.

·       By Default, Auto adjust is ON.

Fig 2.13 Auto adjust profile ON/OFF button

 

Fig 2.14 Original model

 

Fig 2.15 On editing dimension 50 to 100 with auto adjust feature ON

 

Fig 2.16 Edit dimensions with auto adjust feature OFF

 

2.9 Open Mouse Help panel

 

·       Click on Open Mouse Help panel to view the mouse buttons help menu.

 

Fig 2.17 Mouse help panel

 

2.10 Zoom In

 

·       On click, provides zoom in functionality.

Fig 2.18 Zoom in button

 

2.11 Zoom Out

 

·       On click, provides Zoom out functionality.

Fig 2.19 Zoom out button

 

2.12 Zoom All

 

·       On Click, Fits the model to the window.

Fig 2.20 Zoom all button

 

2.13 Zoom Window

 

·       Provides a window to zoom in required features in the model.

·       After clicking Zoom Window, click on screen and drag. This draws a window area which will be zoomed on mouse release.

Fig 2.21 Zoom window button

 

Fig 2.22 Model with zoom window

 

2.14 Move (Pan)

 

·       Hold left mouse button and drag to move the model.

·       On mouse release, Pan is reset. So model is rotated on left click and drag.

Fig 2.23 Pan button

 

2.15 Rotate

 

·       Hold left mouse button and drag to rotate the model.

Fig 2.24 Rotate button

 

2.16 Grid ON/OFF

 

·       Switches the Grid to ON or OFF.

 

Fig 2.25 Grid turned ON

 

3. Plane Section Toolbar

Fig 3.1 Plane section toolbar

 

·       Click on the plane section button in side toolbar to open Plane Section Toolbar.

·       This toolbar has XY plane, YZ plane, ZX plane, Face plane and Invert plane.

·       Create a 3D Model. Then click one of these buttons to view the respective cross sections of the model in their corresponding plane.

 

3.1 XY - Plane

Fig 3.2 XY plane button

 

·       Create a 3D Model.

·       Click on XY–Plane button.

·       A transparent sectional plane appears on the model in XY plane.

·       Click on the plane and move it to view the cross section of the model in XY direction.

·       To exit the planar view, press Esc or ‘X’ button in section toolbar.

·       Refer Fig 3.3.

 

Fig 3.3 XY plane in model

 

3.2 YZ - Plane

Fig 3.4 YZ plane button

 

·       Create a 3D Model.

·       Click on YZ–Plane button.

·       A transparent sectional plane appears on the model in YZ plane.

·       Click on the plane and move it to view the cross section of the model in YZ direction.

·       To exit the planar view, press Esc or ‘ X ’ button in section toolbar.

·       Refer Fig 3.5.

 

 

Fig 3.5 YZ plane on model

 

3.3 ZX - Plane

Fig 3.6 ZX plane button

 

·       Create a 3D Model.

·       Click on ZX–Plane button.

·       A transparent sectional plane appears on the model in ZX plane.

·       Click on the plane and move it to view the cross section of the model in ZX direction.

·       To exit the planar view, press Esc or ‘ X ’ button in section toolbar.

·       Refer Fig 3.7.

 

Fig 3.7 ZX plane on model

 

3.4 Face – Plane

 

Fig 3.8 Face plane button

 

·       Create a 3D Model.

·       Click on Face button in side toolbar à Click on a face of the model to choose the plane direction.

·       A transparent sectional plane appears on the model in selected plane.

·       Click on the plane and move it to view the cross section of the model.

·       To exit the planar view, press Esc or ‘ X ’ button in section toolbar.

·       Refer Fig 3.9.

 

Fig 3.9 Face plane on model

 

3.5 Invert – Plane

 

Fig 3.10 Invert plane button

 

·       Create a 3D Model.

·       Click on Face button in side toolbar à Click on a face of the model to choose the plane direction. Ref Fig 3.11.

·       A transparent sectional plane appears on the model in selected plane.

·       Now Click on Invert button in side tool bar. This inverts the planar view. Ref Fig 3.12.

·       Click on the plane and move it to view the cross section of the model.

·       To exit the planar view, press Esc or ‘ X ’ button in section toolbar.

 

Fig 3.11 Face plane view

 

 

Fig 3.12 Invert plane view

 

4. Page Side Toolbar

Fig 4.1 Page side toolbar

 

·       Multiple Pages/Tab feature is supported in this application.

·       To add a new page, Click ‘ + ’ button or Ctrl + N key.

·       To Switch between pages, click on the respective tab.

·       Each page can have a separate view like Top, Bottom, Left, Right, Front, Back, Default view.

·       Each Page has its own Grid, Models, Rotator position, Feature tree selection, etc.

·       Also, every page can be rotated, moved independent of each other.

·       To close a tab/page Click on ‘ X ’ button in the respective page in side tab.

 

5. File Module Toolbar

 

Fig 5.1 File module toolbar

 

5.1 New

 

Fig 5.2 New button

 

·       Click on New à Adds a new page to the application.

·       New page can also be added by Clicking on ‘ + ’ button in Page Side toolbar or pressing Ctrl + N key.

·       Refer Section 4 for new page addition.

 

5.2 Open

 

Fig 5.3 Open

 

·       Click on Open à File Open dialog box appears à Browse for *.alarvy format file.

·       Revolve Model along with all the sub features are created from the inputs given in *.alarvy file and shown in the current page.

·       Refer section 9 for Alarvy file format (*.alarvy).

 

5.3 Save

 

Fig 5.4 Save file

 

·       Click on Save à File Save dialog box appears à Choose a folder path to save the file.

·       Saves the model data in the current page in *.alarvy format.

·       Refer section 9 for Alarvy file format (*.alarvy).

·       If multiple models exist in the same page, they are saved in the same file.

 

5.4 Save As

 

Fig 5.5 Save As

 

5.4.1 Save As STL

 

·       Click on Save As à STL à File Save dialog box appears à Choose a folder path to save the file as STL.

·       Saves the model in current page in ASCII STL format.

·       In case multiple models are available in current page, below Model dialog is shown. Ref Fig 5.6

·       Check or Uncheck the checkbox next to the models to save them in STL file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

Fig 5.6 Save As multiple model settings

 

5.4.2 Save As STL (Binary)

 

·       Click on Save As à STL à File Save dialog box appears à Choose a folder path to save the file as STL.

·       Saves the model in current page in Binary STL format.

·       In case multiple models are available in current page, above Model dialog is shown. Ref Fig 5.6.

·       Check or Uncheck the checkbox next to the models to save them in STL file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

5.4.3 Save As OBJ

 

·       Click on Save As à OBJ à File Save dialog box appears à Choose a folder path to save the file as OBJ.

·       Saves the model in current page in *.OBJ format.

·       In case multiple models are available in current page, above Model dialog is shown. Ref Fig 5.6

·       Check or Uncheck the checkbox next to the models to save them in OBJ file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

5.4.4 Save As GLTF

 

·       Click on Save As à GLTF à File Save dialog box appears à Choose a folder path to save the file as GLTF.

·       Saves the model in current page in *.GLTF format.

·       In case multiple models are available in current page, above Model dialog is shown. Ref Fig 5.6.

·       Check or Uncheck the checkbox next to the models to save them in GLTF file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

5.4.5 Save As GLB

 

·       Click on Save As à GLB à File Save dialog box appears à Choose a folder path to save the file as GLB.

·       Saves the model in current page in *.GLB format.

·       In case multiple models are available in current page, above Model dialog is shown. Ref Fig 5.6.

·       Check or Uncheck the checkbox next to the models to save them in GLB file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

5.4.6 Save As STEP

 

·       Click on Save As à STEP à File Save dialog box appears à Choose a folder path to save the file as STEP.

·       Saves the model in current page in *.STEP format.

·       In case multiple models are available in current page, above Model dialog is shown. Ref Fig 5.6.

·       Check or Uncheck the checkbox next to the models to save them in STEP file.

·       Multiple models can be saved separately as multiple files or can be saved in single file.

·       By Default, all the models are selected and Single File option is enabled.

 

6. View Module Toolbar

 

Fig 6.1 View toolbar

 

6.1 Undo

 

Fig 6.2 Undo

 

·       Click on Undo à Undoes an operation in the active page only.

·       While sketching a revolve/subsection model, clicking on Undo will remove the last added point.

·       When removing the point, corresponding dimensions are also removed.

·       After creating a revolve/subsection, click on Undo will remove the last added point in the model and shows the sketcher mode again to complete the sketch.

·       After revolve model is created, add sub features like grooves, holes, etc. Now clicking on Undo removes the last added sub feature and the model is redrawn to its previous state.

·       Whenever a feature is removed, its corresponding dimensions are also removed.

·       Entry on the feature tree is also removed.

·       Keyboard shortcut – Ctrl + Z.

 

6.2 Redo

 

Fig 6.3 Redo

 

·       Click on Redo à Redoes an operation in the active page only.

·       While sketching a revolve/subsection model, clicking on Redo will add the last point removed by Undo.

·       When adding the previous point, corresponding dimensions are also added.

·       On a closed revolve model with sub features like grooves, holes, etc, clicking on Undo removes the last added sub feature. Now click on Redo to add removed sub features and the model is redrawn to its previous state.

·       Whenever a feature is added by Redo, its corresponding dimensions are also added.

·       Entry on the feature tree is also restored.

·       Keyboard shortcut – Ctrl + Y.

 

6.3 Clear

 

Fig 6.4 Clear

 

·       Click on Clear à Removes all the models with its feature tree in the active page.

 

6.4 Views

 

Fig 6.5 Views

 

·       Selects the predefined 3D View of the model.

·       Click on Views à Default View.

·       This displays the active page/model in Isometric view.

·       Refer Fig 6.6.

 

Fig 6.6 Default view

 

·       Click on Views à Top View.

·       This displays the active page in Top view i.e., XY Plane and +Z direction.

·       Refer Fig 6.7.

 

Fig 6.7 Top view

 

·       Click on Views à Front View.

·       This displays the active page in Front view i.e., XZ Plane and -Y direction.

·       Refer Fig 6.8.

 

Fig 6.8 Front view

 

·       Click on Views à Right View.

·       This displays the active page in Right view i.e., YZ Plane and +X direction.

·       Refer Fig 6.9.

 

Fig 6.9 Right view

 

·       Click on Views à Left View.

·       This displays the active page in Left view i.e., YZ Plane and -X direction.

·       Refer Fig 6.10.

 

Fig 6.10 Left view

 

·       Click on Views à Back View.

·       This displays the active page in Back view i.e., XZ Plane and +Y direction.

·       Refer Fig 6.11.

 

Fig 6.11 Back view

 

·       Click on Views à Bottom View.

·       This displays the active page in Bottom view i.e., XY Plane and -Z direction.

·       Refer Fig 6.12.

 

Fig 6.12 Bottom view

 

7. Settings and Help Toolbar

 

Fig 7.1 Settings and help toolbar

 

 7.2 Settings

 

Fig 7.2 Settings button

 

·       Click on Settings icon à Opens Settings Panel.

·       Settings for Grid, Theme, Save As file options, arrow dimensions and Turn module features are available.

·       Click on Save in settings panel to save the changes made by user.

·       Click on Reset to reset the changes made by user to default values.

·       Click on Cancel to discard the changes and close the settings panel.

 

7.2.1 Grid Settings

 

Fig 7.3 Grid settings

 

·       Click on Settings icon à Opens Settings Panel à Expand Grid Settings.

·       Specifies below settings for Grid.

·       Unit à Specifies Unit. By default, mm is selected.

·       Length(x) à  Specifies the grid length in X direction. Default value is set to 1500. This value is editable.

·       Width(y) à  Specifies the grid length in Y direction. Default value is set to 1000. This value is editable.

·       Step à Specifies the distance between two line-segments in X direction or Y direction. Default value is 5. This value is editable.

 

7.2.2 Theme Settings

 

Fig 7.4 Theme settings

 

·       Click on Settings icon à Opens Settings Panel à Expand Theme Settings.

·       Specifies Theme settings for the application.

 

Select Theme à

·       Applies the selected theme to the application.

·       Click on the dropdown to choose the available theme options.

·       Changing the theme changes the colour of Toolbar, Button hover, active button, text, background and Grid.

·       Standard theme attributes cannot be changed.

·       To create a Custom theme à Choose Custom in dropdown à change the colour of all attributes, click on Save button next to the dropdown à Give a name to this custom themeà Click on ü.

 

Toolbar Colour à

·       Specifies the colour of the Toolbar, Settings panel and Side toolbar.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the toolbar colour value à Opens Colour palette à Pick a colour for the toolbar.

·       Toolbar colour of Standard Themes cannot be edited.

 

Button Hover Colour à

·       Specifies the colour of the Buttons on Hovering in the toolbars, side toolbars, page tabs.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the colour value à Opens Colour palette à Pick a colour for the button hover.

·       Button Hover colour of Standard Themes cannot be edited.

 

Active Button Colour à

·       Specifies the colour of the active buttons in the page.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the colour value à Opens Colour palette à Pick a colour for the active button.

·       Active Button colour of Standard Themes cannot be edited.

 

Text Colour à

·       Specifies the colour of the text in Toolbar, Settings Panel and Side toolbar.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the colour value à Opens Colour palette à Pick a colour for the Text.

·       Text colour of Standard Themes cannot be edited.

 

Toolbar Text à

·       Specifies whether text in Toolbar should be displayed or not.

·       By Default, Toolbar text is set to ‘Show’.

 

Text Size à

·       Specifies the size of the text in Toolbar, Settings Panel and Side toolbar.

·       Default size is 12.

·       Size is editable for all themes.

 

Background Colour à

·       Specifies the background colour of the application.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the colour value à Opens Colour palette à Pick a colour for the Background.

·       Background colour of Standard Themes cannot be edited.

 

Grid Colour à

·       Specifies the colour of grid line segments.

·       This is editable but on saving, it will be saved as a new Custom theme with a user specified name.

·       Click on the button next to the colour value à Opens Colour palette à Pick a colour for the Grid lines.

·       Grid line colour of Standard Themes cannot be edited.

 

7.2.3 Save As Settings

 

Fig 7.5 Save As settings

 

·       Click on Settings icon à Opens Settings Panel à Expand Save As GLTF / GLB Settings.

·       Specifies Saving options for GLTF / GLB files.

·       Revolve model in active page can be saved by File Toolbar à Save As à GLTF or GLB. Refer Sec 5.4.4, 5.4.5.

·       3D à Specifies whether 3D Solid Model should be saved in GLTF / GLB File. By Default, it is ON, saves the 3D Model.

·        Sketch à Specifies whether the 2D Sketch of the Model should be saved in GLTF / GLB File. By Default, it is ON, saves the 2D Sketch.

·       Dimensions à Specifies whether the Dimensions of the Model should be saved in GLTF / GLB File. By Default, it is ON, saves the Dimensions.

 

7.2.4 Arrow dimensions Settings

 

Fig 7.6 Arrow dimension settings

 

·       Click on Settings icon à Opens Settings Panel à Expand Arrow Dimension Settings.

·       Specifies the Size of the arrows and Text in Dimensions.

·       Arrow Head Length à Set the Head Length size of the arrow. Default is 15.

·       Arrow Head Width à Set the Head Width size of the arrow. Default is 15.

·       Dimension Text Size à Sets the size of the text in the dimensions. Default is 12.

 

7.2.5 Turn module Settings

 

Fig 7.7 Turn module settings

 

·       Click on Settings icon à Opens Settings Panel à Expand Turn Module Settings.

·       Specifies the settings of various turn module features like Groove, Fillet, Chamfer, Hole and Step.

 

7.2.5.a Groove Settings

 

Rectangular Groove à

Fig 7.8 Rectangular groove

 

·       Specifies the dimensions of Rectangular Groove.

·       Turn toolbar à Groove à Rectangular Groove adds the groove to the model.

·       Height à Sets the Height of the rectangular groove. Refer Fig 7.8.

·       Base width à Sets the base width of the rectangular groove. Refer Fig 7.8.

 

Trapezoidal Groove à

 

Fig 7.9 Trapezoidal groove

 

·       Specifies the dimensions of Trapezoidal Groove.

·       Turn toolbar à Groove à Trapezoidal Groove adds the groove to the model.

·       Refer Fig 7.9 for dimensions.

·       Height à Sets the Height of the Trapezoidal groove.

·       Base width à Sets the base width of the Trapezoidal groove.

·       Angle right à Sets the angle of inclination between the right edge and base edge.

·       Angle left à Sets the angle of inclination between the left edge and base edge.

 

Filleted Rectangular Groove à

 

Fig 7.10 Filleted rectangular groove

 

·       Specifies the dimensions of Filleted Rectangular Groove.

·       Turn toolbar à Groove à Filleted Rectangular Groove adds the groove to the model.

·       Height à Sets the Height of the Filleted rectangular groove. Refer Fig 7.10.

·       Base width à Sets the base width of the Filleted rectangular groove. Refer Fig 7.10.

·       Fillet radius à Sets the fillet radius of the groove.

 

Filleted Trapezoidal Groove à

Fig 7.11 Filleted trapezoidal groove

 

·       Specifies the dimensions of Filleted Trapezoidal Groove.

·       Turn toolbar à Groove à Filleted Trapezoidal Groove adds the groove to the model.

·       Height à Sets the Height of the groove.

·       Base width à Sets the base width of the groove.

·       Fillet radius à Sets the fillet radius of the groove.

·       Angle right à Sets the angle of inclination between the right edge and base edge.

·       Angle left à Sets the angle of inclination between the left edge and base edge.

 

7.2.5.b Fillet Settings

 

Fillet Radius à

 

Fig 7.12 Fillet radius setting

 

·       Specifies the dimensions of Fillet.

·       Turn toolbar à Fillet à adds fillet at the selected edge/point in the model.

·       Sets the default radius of the fillet.

 

7.2.5.c Chamfer Settings

 

Fig 7.13 Chamfer settings

 

Chamfer leader dimensions à

·       Specifies whether the leader dimensions of Chamfer should be enabled or not.

·       Refer Fig 7.13 for settings.

·       By default, it is ON.

·       Refer Fig 7.14 – leader dimensions are OFF.

·       Refer Fig 7.15 – leader dimensions are ON.

 

Fig 7.14 Leader dimensions OFF

 

Fig 7.15 Leader dimensions ON

 

Chamfer LL à

·       Refer Fig 7.13 for settings.

·       Sets the dimensions of L1 and L2 in chamfer type L1 X L2.

·       L1 and L2 are the distance between the intersecting points to the edges in the model.

·       Default value is 5 x 5.

·       Refer Section 1.6.i for details on L1 and L2 in L1 X L2 chamfer.

 

Chamfer SLA à

·       Refer Fig 7.13 for settings.

·       Sets the dimensions of Slant length and angle in chamfer type CL X Ꝋ.

·       Refer Section 1.6.iii for details on slant length and angle in CL X chamfer.

·       Default value of slant length is 5 and angle is 45.

 

Chamfer LA à

·       Refer Fig 7.13 for settings.

·       Sets the dimensions of previous length(L1) and angle in chamfer type L1 X Ꝋ.

·       Refer Section 1.6.ii for details on L1 and angle in L1 X chamfer.

·       Default value of L1 is 5 and angle is 45.

 

7.2.5.d Hole Settings

 

 

Fig 7.16 Hole settings

 

Hole à

·       Refer Fig 7.16 for settings.

·       Sets the Hole diameter and Hole Depth for the default Hole type.

·       Refer Section 1.7.ii for details on Hole type.

 

Tapered Hole à

·       Refer Fig 7.16 for settings.

·       Sets the Hole Top diameter, Hole Depth, Hole bottom diameter and taper cone angle for the Tapered Hole type.

·       Refer Section 1.7.ii for details on Tapered Hole type.

 

Counter Sink Hole à

·       Refer Fig 7.16 for settings.

·       Sets the Counter Sink angle, Counter sink diameter, Hole Depth and Hole diameter for the Counter Sink Hole type.

·       Refer Section 1.7.ii for details on Counter Sink Hole type.

 

 

Fig 7.17 Hole settings

 

Counter Bore Hole à

·       Refer Fig 7.17 for settings.

·       Sets the Counter bore diameter, Counter bore depth, Hole Depth and Hole diameter for the Counter Sink Hole type. Refer Section 1.7.ii for details on Counter bore Hole type.

 

Counter Drill Hole à

·       Refer Fig 7.17 for settings.

·       Sets the Counter drill diameter, Counter drill depth, Counter sink diameter, counter drill angle, Hole Depth and Hole diameter for the Counter drill Hole type.

·       Refer Section 1.7.ii for details on Counter drill Hole type.

 

Circular Pattern Hole à

·       Refer Fig 7.17 for settings.

·       Sets the default number of holes in Circular Pattern hole.

·       By default, number of holes set is 5.

·       Refer Section 1.7.iii and Fig 1.7.8 for details on Circular Pattern Hole type.

 

7.2.5.e Step Settings

 

Step à

Fig 7.18 Step settings

 

·       Refer Fig 7.17 for settings.

·       Sets the Height, Base width and angle of Step.

·       Refer Fig 7.18 for the dimensions in Step.

·       Refer Section 1.4 and Fig 1.4.2 for details on Step feature.

 

7.3 Help

Fig 7.19 Help button

 

7.3.1 Help

·       Opens help file for user understanding.

 

7.3.2 Tutorial Videos

·       Opens a link to tutorial videos.

 

7.3.3 About

·       Opens the user agreement, privacy policy, disclaimer, acknowledgement and other information of Alarvy Cad application.

 

8. Special features

AlarvyCAD application has below special features

·       Rotator

·       Feature tree

·       Contextual Help

 

8.1 Rotator

Fig 8.1 Rotator cube

 

·       Rotator cube is positioned at top right corner of the page.

·       It specifies the current orientation of the model and grid in the current page.

·       Rotator has axis helpers – X, Y, Z starting from its centre.

·       It also has view helpers (Spherical objects at the end of axis helpers). When clicked on the X, Y or Z balls, rotates the model in that direction.

·       On clicking the axis balls, say X, rotates the view by 90 degree in X direction.

·       There are 6 available default views with Rotator – Top, Front, Left, Right, Back, Bottom.

·       Click on a view in cube face to see the respective Top or Bottom or Front view, etc of the 3D Model.

·       Click on the Rotator cube and drag to see the corresponding rotated view of the model/grid.

·       Rotating the model will rotate the rotator cube also to match the orientation.

·       On multiple Page switch, Orientation of Rotator cube will be updated with the orientation of the model as in active page.

 

 8.2 Feature Tree

 

·       Feature tree is displayed at top left corner next to page tab.

·       It shows all the features and models added in the current page.

·       Refer Fig 8.2.

·       Selecting an entry in feature tree, highlights the corresponding feature in the model.

·       To delete a feature in the model, select the same in feature tree and Click Delete in toolbar or Delete key in keyboard.

 

Fig 8.2 Feature tree

 

8.3 Contextual Help

 

·       Contextual help is displayed at the bottom of the page.

·       Refer highlighted part in Fig 8.3.

·       It gives information to user on every action currently done on the screen.

·       For example – When Grid ON/OFF button is clicked, it displays “Show grid is turned ON”.

·       Contextual help also instructs the user on what to do next when specific feature is selected.

·       For example – Ref Fig 8.3, When Revolve is clicked, before placing the first point, it instructs the user to add the first point or on how to exit sketcher mode. Also, on mouse move it displays the current position.

·       Contextual help also displays the error messages.

·       Refer Fig 8.4 for example – When chamfer dimensions were edited to incorrect values, message in figure was displayed.

 

Fig 8.3 Contextual help

 

Fig 8.4 Error message in contextual help

 

9. Alarvy File Format

 

·       Alarvy file format is in the form of json file.

·       Click Save in File module toolbar to save the active page Turn part in *.alarvy file.

·       Click Open in File module toolbar to open the *.alarvy file and render the Turn part in UI.

 

Fig 9.1 *.alarvy file top level

 

·       Refer Fig 9.1 for *.alarvy file top level json structure.

·       Contains the following fields –

o    id – unique id of the revolve model,

o   modeler – name of the modeler, here it is ‘turn’,

o   module name,

o   datatype - ‘multibodySolid’ (as it can contain multiple revolve models),

o   unit - unit used in application,

o   version number,

o   parts – holds data of multiple models in the current page,

o   subassemblies and

o   assembly information

 

9.1. Parts

 

·       Holds the model data of all the revolve model in the active page.

·       Multiple models are stored as separate array.

·       Refer Fig 9.2 for multiple model example.

·       Each part model has below fields –

o   Id – id of the part,

o   Modeler – name of the modeler, here ‘turn’,

o   Module – name of the module, ‘revolve’,

o   Datatype – solid model,

o   Unit – unit used in application,

o   Profile – Holds information on Combined sketch of individual revolve models including all sub features,

o   Features – Holds information on revolve sketch only,

o   Hole features – Holds information on Hole features in the revolve model,

o   Threads – Holds information on Threads in the revolve model,

o   Dimension positions.

 

Fig 9.2 – Example of multiple models in parts

 

9.1.1 Profile

 

·       Holds the combined sketch information of the profile.

·       Refer Fig 9.3 for Profile information.

·       It Holds Sketch data for the whole profile including all the points and edges added by the sub features also.

·       It has following properties

·       Sketchtype – revolve models contains ‘closed’ sketch.

·       Points – Array of all points in the revolve model. Each point has X, Y, Z coordinates.

·       Edges – Array of all edges in the revolve model.

·       Each edge has an id, start point, end point, type - arc or line,

arctype - if edge has arc, type is specified,

hasthread – whether it has a thread or not,

edited information, constraint.

·       Other edge data are available based on its type

 

 

Fig 9.3 Profiles

 

9.1.2 Features

 

Fig 9.4 Features

 

·       Holds feature wise information.

·       Revolve feature holds feature type, points, edges and its sub features. Refer Fig 9.4

·       Each sub feature holds its own data like id, feature type, feature name, feature specific data and its sub features

·       Refer Fig 9.5 for Chamfer sub feature and Fig 9.6 for Subsection feature as sample structures

 

Fig 9.5 Chamfer sub-feature data

 

Fig 9.6 Subsection sub-feature data

 

9.1.3 Hole Features

 

·       Holds data of all Hole features added to the revolve model. Refer Fig 9.2.

·       Each hole feature contains id, type, feature type, feature name, penetration type, bottom type, orientation type, pattern type, count, hole diameter, hole depth, PCD – pitch circle diameter, position, rotation, quaternion, surface normal, locating plane normal, hole points, hole segments, parent edge, parent edge id, parent line index, sub features, edited info.

·       Other parameters depend on the hole type.

 

9.1.4 Threads

 

·       Holds data of all Threads features added to the revolve model. Refer Fig 9.2.

·       Each thread contains id, type, feature type, feature name, draw actual threads, thread standard, shank position, thread length, shank length, base diameter, minor diameter, pitch, designation index, designation, thread sketch feature, thread start point, parent edge index, parent edge, parent id and edited info.

 

9.1.5 Dimension Positions

 

Fig 9.7 Dimension positions

 

·       Holds data of all dimensions added in revolve model. Refer Fig 9.2, 9.7.

·       Dimensions are grouped as follows

o   lengthDimPositions – all Line dimensions,

o   diaDimPositions – all circular edges diameter dimensions,

o   filletDimPositions – all fillets dimensions,

o   arcDimPositions – all arcs dimensions,

o   chamferDimPositions – all chamfer features dimensions,

o   holeDimPositions – all hole features dimensions,

o   threadDimPositions – all thread features dimensions.