Sometimes, the surfaces used to extract parting lines can contain abnormalities or they may not mate correctly. This can occur when surfaces are imported from a neutral file such as IGES. VX offers many topology healing commands but gaps between parting lines can still occur at times.  This command can be used to fill those gaps.

 

This command can also be used to bridge known gaps between parting lines such as the example shown below. On this propeller design, the Parting Lines from Silhouettes command created all of the necessary parting lines except for those that are needed to span along the central hub. This gap occurs where each of the three blades are attached to the hub. You can use this command to bridge all three gaps at the same time with curvature continuous parting lines that span along the surface of the hub.

 

Filling Gaps between Two (or more) Parting Lines

Final Core/Cavity Plates using Filled Parting Lines

 

 

 

Gaps in topology (i.e., how vertices, edges and faces connect) can sometimes occur when parts are imported from other modeling applications through the use of neutral data formats such as IGES. VX can fill many of these gaps if they are surrounded by a closed loop of edges.

 

In the part on the left shown below, 253 gaps were identified using the Inquire Open Edges command. The gaps (i.e., holes in the part) appear red because the back faces of other faces are showing through the gaps.  You can use this command to fill these gaps automatically.

 

When prompted to select edges, middle-click to select the entire part. The new faces shown in green in the part on the right are created. Using the Inquire Open Edges command again reveals that there are no longer any open edges.  Remember, as long as there are boundary edges around the gap, it can be closed.

 

Before

After

 

 

 

The Extrude Shape command can be used early in a design to create the basic shape of a part or to create basic features by adding or removing extruded material. In the application shown below, an extruded shape is added to create the knob mount of the fishing reel arm. A datum plane is created ahead of time to locate the feature. During the command, a sketch is created to define the profile of the extruded shape. Refer to the sequence of figures below.

 

 

 

 

This command can be used early in a design to create the symmetrically revolved shape of a part. It can encompass much geometry into a single feature including fillets. While this command is used early, fillets are considered finishing features and are typically applied late in the design. The preference is yours. You can also add and remove material using this command by selecting the appropriate icon from Options Menu.

 

 

 

In the example shown above, a sketch is used to revolve the basic shape of this part.  In this case, fillets are included in the sketch and thus in the feature.  The revolve axis is shown with a red arrow. The axis can be a line in the sketch as shown or the sketch can be open as long as both ends contact the axis.

 

There are different ways you can edit the feature. You can modify a dimension value (without activating the sketch) and then regenerate the part. You can also redefine the feature. You can execute this command from the Edit>History Operations menu or by right-clicking on the feature name listed in the History Manager(Ctrl+H).

 
 

 

The Sweep Shape command can create a wide range of shapes that provide the basis for many complex parts such as propellers, fans and other ergonomic shapes. The command's extensive controls for position, orientation, scale, twist and variable attributes can be combined with VX's expression evaluator to derive formulae-based shapes such as turbine blades.

 

Sweep Shape - Linear Twist

Sweep Shape - Linear Scale
 

 

 

 

Using the Extrude Sheet Metal command, your initial shape does not have to be flat as shown in this figure.  

 

You can also use this command to create the basic shape by sketching the cross-section of the sheet metal part.  The sketch can include fillets but they will have to be marked as bends after the feature is complete.  The material thickness can also be implied using an open profile (i.e., only one side of the cross-section needs to be sketched).

 

The series of illustrations below shows how this command can be used to design the initial shape of a sheet metal part within the context of an assembly using a mating component as a reference.

 

 

 

 

Figure 1 - A new assembly is created and an existing component is inserted at the default origin.  In this example, an automotive reservoir bottle is used.  Next, a new component is inserted.  This means that a new part is created within the context of the assembly and is activated.  

 

Now the basic shape of the part can be created using the Extrude Sheet Metal command.  During the command, a sketch is inserted on the default XZ datum plane and is activated.  Refer to Figure 1 above.

 

 

 

 

Figure 2a and 2b (above) - To begin the sketch, Quick Draw is used to create the two Lines A and B.  During the command, the F7 key (i.e., extended pick) is pressed while selecting endpoints A, B, C and D.  

 

This creates external references (red triangles) between the sketch and the reservoir bottle component.  If the bottle changes, the sketch will also.

 

 

Figure 3 (right) - With Lines A and B drawn, the sketch isolated visually using the Show Target command.  A fillet is then added between the lines.  Using the Trim/Extend Curves (2D) command, line A is extended opposite the fillet.

 

 

Figure 4a and 4b - Using Quick Draw, perpendicular Line C and parallel Line D are drawn with the help of Smart Pick.  Line C begins at the end of Line B and stops when Smart Pick determines that it is perpendicular to Line B and vertical with its midpoint.  

 

Line D begins at the end of Line C and stops when Smart Pick determines that it is parallel to Line B and vertical to the endpoint of Lines B and C.  Quick Draw and Smart Pick can be used to draw and position a wide range of geometry.

  

 

 

 

 

Figure 5 (top left) - Fillet are created between Lines C, C and D.  Since we are only sketching one side of the cross-section, the fillet radii reflect one inner and one outer bend radius.  The geometry is now complete and the sketch is exited.

 

Figure 6 (top right) - When you exit the sketch, the Extrude Sheet Metal command is resumed.  Since the sketch is an open profile, you are asked to locate the interior of the sketch.  A point on the sketch is selected and the arrow is dragged to indicate the interior direction.

 

 

 

 

Figure 7 (above) - Now the command is asking for the start and the end of the extrusion.  On the Optional Inputs section of the Options Form the Offset is set to Shrink/Expand and the 1st Offset value is set to 1.0.  

 

This is why we only had to sketch one side of the cross-section.  The thickness is implied during the command.  Notice that the offset is shown in the preview.

 

Figure 8 (right) - The final shape of the part is shown using the Extrude Sheet Metal command.  As you can see 80% of the part is created using this command.

 

 

 

If you have parts that are dimensionally similar, VX can derive a family of parts from a single part model.  This eliminates the need to have many similar models on hand.  If you need a part from the family, it can be derived on-the-fly at any time.  

 

VX accomplishes this with the use of driving parameters.  The figures below illustrate the basic process.  Guidelines, tips and suggestions are also provided along the way.

 

 

Figure 1 - The "Parent" Part

 

The process begins by loading any part that contains dimensions that can be modified to create another version of the part.  In this application, the Eye Rod shown above contains four dimensions that are used as driving parameters.

 

 

 

 

Figure 2 - Adding Name Tags to Dimensions

The first step is to attach name tags to those dimensions that we want to drive the part (Attributes > Tags).  In the Options Form shown to the right, we are attaching the name

"Rod_Length" to the 95.00 dimension shown in Figure 1 above.  The command is repeated for the remaining three dimensions (i.e.,  Hook_Radius - R10.00,  Blend_Radius - R26.00 and Rod_Radius - R3.00).

 

 

 

 

Figure 3 - Setting up Driving Dimensions

 

 

Once all of the dimensions are tagged, you need to display the Part Attributes Form (Attributes > Part).  On the Driving Parameters tab you need to assign each dimension as a driving parameter.  This is done by selecting the first button and then selecting the dimension from the part.  The dimension name will appear on the button and the value will appear in the input field.  This is done for each dimension.

 

 

 

 

Once the part attributes are saved (pick OK), the part needs to be saved and then closed.  In our example, the part name is Eye Rod 1042256.  This will return you to the Object Level where the Root Object Browser is displayed.

 

There are previewing options located at the bottom of the Root Object Browser.  You can preview graphics, attributes and assemblies.  To derive a family of parts, check the box next to Attributes.  When you select a part from the list, its part attributes are displayed (see Figure 4).

 

 

Figure 4 - Previewing Attributes

 

 

When the part is selected from the Root Object Browser, its part attributes are displayed.

 

 

 

Figure 5 - Deriving a New Part

The Driving Parameters tab previews the driving parameters that we assigned to key dimensions in the part.  You can enter the desired values for each parameter and then pick the Derive new part button.  You are asked for a name of the new part.  The new part is calculated from the parameters of the previewed part.  In this case we are deriving a family of parts from our parent part "Eye Rod 1042256."

 

Create new file

When you enter a name for the new part, you can choose to create a new VX file at the same time. Otherwise the part will be added to the active file.

 

 

(a)

 

(b)

 

(c)

 

(d)  

 

(e)

 

Figure 6 - The Family of Parts

When a new part is derived from the parent part, it is added to the active VX file and shown in the Root Object Browser.  We derived the four parts shown in Figures 6b through 6e above from the parent part shown in 6a.  This is referred to as a family of parts.  They are listed in the Root Object Browser.

 

 

 

 

 

You can make smooth surfaces while still having the simplicity of drawing with arcs by using Designer Arcs.  A Designer Arc is a NURB curve that matches the tangency of the arc but has zero curvature at the end points. If the Designer Arc is inserted with the Fillet 2 Curves (3D/2D) command, it will match the curvature of the neighboring curves.

 

 

 

When a Designer Arc is drawn, the circular arc on which it is based is also drawn in a "dotted" font. This is used as a visual clue that this non-circular NURB curve still has the properties of an arc (i.e., it can be driven through the constraint system with a radius dimension).

 

 

 

 

 

 

The example history tree here shows three operations that are derived from the Custom Input operation called MyPin.  The first two shape operations Cylinder1_Base and Cylinder2_Base contain inputs derived from MyPin.  The third operation Boolean1_Add joins the two shapes into the final pin.  These four operations are used to create a Custom Feature.

 

Remember that the derived operations must directly follow the Custom Input operation.  Let's step through the first operation Cylinder1_Base to see how it's done.

 

1. The first operation is the Basic Cylinder Shape command.  Invoke the command and the Options Form shown below is displayed.
   
   
   
   
    

2. First select the Base method icon (if it's not already the default).
    

3. You are then prompted for the center of the cylinder.  Make sure the Text Input Field is active.  The center location will be derived from the Point input of the Custom Input operation MyPin.
    

4. Display the History Manager.
    

5. Right-click on MyPin in the History Manager and select Open/Close.  This will expand the operation.  Skip this step if MyPin is already open.
    

6. Now right-click on Point : on entity (0,0,0) and select Send.  This will send the Point input from MyPin directly to the Text Input Field.  This is how the feature operations will derive input from the Custom Input operation.
    

The next two prompts Radius and Length are indirectly derived from MyPin using expressions.
 

7. When prompted for the radius of the cylinder, right-click in the graphics window and select Expression.  This will display the Input Expression Form.  See Using Command Line Expressions for more about this form.
    

8. Make sure the Expression field is active.  Now, from the History Manager right-click on Diameter : 20 mm and select Send.  This will send the Diameter input from MyPin directly to the Expression field (see below).

 

 

 

 

9. Now add /2 at the end of the Expression field and then pick OK (see above).  This sets up an expression (Diameter/2) whose value is indirectly derived from the Custom Input operation.  This value is assigned to the radius prompt for the Basic Cylinder Shape command.
    

The link between Radius and the Custom Input MyPin is not explicitly shown on the History Manager.  If you right-click on Radius in the History Manager and select Edit, the Input Expression Form is displayed with the original expression used to define Radius.  There you can see that the expression is linked to the Diameter field of MyPin (Field ID #3).

 

10. Perform the same procedure when prompted for the length of the cylinder.  But this time right-click on Length : 50 mm and select Send.  Then add *-1 at the end of the Expression field (see below) and pick OK.  This sets up an expression (Length*-1) whose value is again indirectly derived from the Custom Input operation.  This value is assigned to the length prompt for the Basic Cylinder Shape command.

 

 

 

 

11. Finally, use the Align plane option of the Basic Cylinder Shape command.  Selecting the Define button, the command prompt says "Select alignment plane" and the Text Input Field is again active.
     

12. Now go back to MyPin in the History Manager again.  Right-click on Plane : XY and select Send.  Again, this will send the Plane input from MyPin directly to the Text Input Field as input to the Align plane option.
     

13. Pick OK from the Options Form and the first operation Cylinder1_Base is now complete.
     

14. The second operation Cylinder2_Base is also the Basic Cylinder Shape command used in a similar manner.  Refer to the history tree example above to see how certain inputs are derived from the MyPin Custom Input operation.
     

15. Finally, the last operation Boolean1_Add is the Combine Shapes command.  During this command, the two previous shapes Cylinder1_Base and Cylinder2_Base are selected (from the graphics window) and then added together.
    
    The part looks like the figure below.  You are now ready to create a Custom Feature.  See Insert Custom Feature to continue this example.

   

 

 

Creating Custom Inputs and Custom Features are the first steps toward creating your own Custom Feature library.  The process is quite simple and uses the 3D clipboard options of the Cut and Paste History commands.

 

1. First, active the part that contains the Custom Feature that you want to add to the library.
    

2. Display the History Manager, right-click on the Custom Feature operation and select Copy.  Alternately, you can press (Ctrl+C) and then select the operation (or select the feature itself).

 

 

Copy a Custom Feature from the History Manager

 

 

Before you complete the copy command, notice the Options Form.  It has a section called File/Part.  This is used to save the active 3D clipboard to a VX file.

 

 

3. The File field will default to the active file.  You can use this file to contain your Custom Feature library or you can select the folder icon and use the File Browser to select another VX file.
    

4. Enter a name for the Custom Feature in the second field on the Options Form.  Make the name descriptive.  You will select this name when you paste the Custom Feature into other parts.
    

5. Pick OK to complete the copy command.

 

Repeat this procedure every time you have a Custom Feature that you want to add to the library.

 

6. Now open a VX file and activate a part that you want to receive the custom feature.
    

7. Right-click in the graphics window and select Paste or simply press (Ctrl+V).
    

8. An Options Form similar to the one used during the Copy command is displayed.
    

9. For the File, select the folder icon to locate and select the VX file that you saved your Custom Feature 3D clipboard in.  All of the Custom Features in the file (i.e., the Custom Feature Library) will be listed.
    

10. Select the Custom Feature that you want to paste and then pick OK.

 

 

 

 

The Options Form for the Custom Input operation created for the Custom Feature is displayed and you are prompted for the required input.  In the example shown above we are pasting the Custom Feature called MyPin.  Refer to the Insert Custom Input command for more about creating the operations required for a Custom Feature.

 

11. Here are our required Custom Inputs (refer to the figure above):

 

• Select the insertion plane to locate the pin.

• Select a point to position the pin.

• Enter the diameter of the pin.

• Enter the length of the pin.

 

12. Pick OK to paste the Custom Feature into the active part.  It will now show up in the History Manager.  If you want to access the sub-operations of the Custom Feature, right-click on it in the History Manager and select Explode.