Creating a cross part parametric pattern

Published date: 2001-02-07

ID: TS64098

Applies to: Mechanical Desktop® Release 4

Issue

You need to create a pattern on parts (for example, screws) that matches features on another part (for example, a hole pattern).

Solution

Use the following procedures to create a cross part parametric pattern:

First create some global variables that will control the number of features/parts and the spacing between these features.

  1. Type amvars on the command line and press ENTER.
  2. Choose New and type X (number of columns) in the Name field, type 2 in the Equation field and choose OK.
  3. Choose New again and type XD (distance between the columns) in the Name field, type 3 in the Equation field, and choose OK.
  4. Choose New again and type Y (number of rows) in the Name field, type 2 in the Equation field, and choose OK.
  5. Choose New again and type YD (distance between the columns) in the
  6. Name field, type 4 in the Equation field, and choose OK.

Once you have created all of the necessary global parameters as described in the preceding procedure, you will have to create two new parts. In this example, you will create an extruded cylinder to represent a bolt.

Create a plate

  1. Type amnew on the command line and press ENTER. Select P for part and enter PLATE as the part name.
  2. Use the REC command to create a rectangle measuring 8 x 10.
  3. Type amprofile on the command line and press ENTER, select the rectangle and press ENTER again.
  4. Use the AMPARDIM command and place a dimension on both sides of the rectangle to make sure they are 8 x 10.
  5. Type amextrude on the command line and press ENTER, then choose OK to extrude the profile into a solid.
  6. Type amhole on the command, press ENTER, and choose OK to accept the default values.
  7. Pick two corner edges of the plate from which to place the hole.
  8. Drag the cursor out about 1 x 1 and click to place the hole. Confirm the hole position by entering a value of 1 for both offsets at the command prompt.
  9. Exit the AMHOLE command.

Create a bolt

  1. Type amnew on the command line and press ENTER.
  2. Select P for part and enter BOLT as the part name.
  3. Use the CIRCLE command to create a circle .5 in diameter.
  4. Type amprofile on the command line and press ENTER, select the circle and press ENTER again.
  5. Use the AMPARDIM command and place a dimension on the diameter of the circle to make sure the diameter is .5.
  6. Type amextrude on the command line and press ENTER, then choose OK to extrude the profile into a solid.

Now that you have created the parts, you can form the cross part parametric pattern. First, you have to create a pattern of hole1 in the part named PLATE.

In the browser, double-click the part named PLATE to make it active.

  1. Type ampattern on the command line and press ENTER.
  2. When prompted to select the feature to be patterned, select an edge on hole1 when only hole1 is highlighted and press ENTER to accept.
  3. In the Pattern dialog box, type X in the Instances field and XD in Spacing field for the Column Placement.
  4. Type Y in the Instances field and YD in Spacing field for the Row Placement.
  5. Choose OK in the Pattern dialog box to create the pattern.

Next, you will create a pattern of the bolt that matches the pattern or hole1 created in the preceding procedure.

  1. In the browser, double-click the part named BOLT to make it active.
  2. Type ampattern on the command line and press ENTER.
  3. When prompted to select the feature to be patterned, select any edge on the part as this part only has the base feature. Note: In parts with multiple features every feature you wish to make part of the pattern must be selected.
  4. In the Pattern dialog box, type X in the Instances field and XD in Spacing field for the Column Placement.
  5. Type Y in the Instances field and YD in Spacing field for the Row Placement.
  6. Choose OK in the Pattern dialog box to create the pattern.

Now you will constrain the part named BOLT to the pattern in the part named PLATE.

  1. Type aminsert on the command line and press ENTER.
  2. Select the bottom circular edge on one of the cylindrical occurrences in the part named BOLT (accept the constraint when the arrow points in the desired direction).
  3. Choose the corresponding hole in the part named PLATE (accept the constraint when the arrow points in the corresponding direction) and accept the default 0 distance offset.
  4. Type aminsert on the command line and press ENTER.
  5. On the part named BOLT, select the bottom circular edge on the cylindrical occurrence diagonally opposite to the one you selected in step 2 (accept the constraint when the arrow points in the desired direction).
  6. Choose the corresponding hole in the part named PLATE (accept the constraint when the arrow points in the corresponding direction) and accept the default 0 distance offset.

Now that the bolt pattern has been constrained to match the hole pattern, you can make both of these change together.

  1. Type amvars on the command line and press ENTER.
  2. In the Design Variables dialog box, select the Global tab.
  3. In the row for the variable X, double-click the current value of 2, enter a new value of 3 and press ENTER.
  4. In the row for the variable XD, double-click the current value of 3, enter a new value of 4 and press ENTER.
  5. Choose OK to exit the Design Variables dialog box.

You can now see that both the hole pattern and the bolt pattern have increased in number, and the spacing has changed as well as well.