How to Create Dimension in NX PMI (Product and Manufacturing Information) |Siemens NX 2206
There are many dimension types in PMI operate and they are essentially similar to the dimensioning commands in the Drafting and Sketching applications.
Before selecting the dimension feature be sure to set the model view on which you want to place your dimension.
This helps to organize your dimensions.
For this lesson, expand the Model Views node on the Part Navigator and make sure the Trimetric model view is set as the Work view.
Make sure to do this every time you place a PMI note, dimension or feature on a part model.
The following video and steps showcase the procedure on how to create and add dimensions to a model within NX PMI.
Follow the below steps to know How to Create Dimension in NX PMI
Step 1
select PMI Tab > Dimension Group > Rapid to activate the Rapid Dimension dialog.
Step 2
In the Orientation drop-down pane, you can define the orientation plane or lock it for subsequent dimensions you create.
When you define the dimension, the orientation plane is inferred and you can select an alternate plane.
Step 3
In the Measurement pane, ensure the Method drop-down is set to Inferred.
Step 4
The Select First Object selection step should be selected in the References pane – pick one of the hole arc centers as shown in the image below.
You can also hover over the arc center and right click for a pop-up menu and select from List… and the QuickPick dialog appears allowing you to choose a specific object.
Step 5
The Select Second Object selection step highlights – pick the other hole center as shown in the image below. Be sure to pick the Arc Center. Picking the edge infers a diametral dimension and instead highlights the Specify Location selection step.
Step 6
Make sure to select the correct plane as shown below. Under Orientation section you can select the Alternate Plane button to switch planes.
Step 7
Drag it out to open area away from the part model as shown then right-click and select Edit to display a Text window along with access handles.
Step 8
Set the Method drop-down to Point-to-Point.
Set the Tolerance drop-down to No Tolerance.
Ensure the Orientation drop-down is set to Horizontal Text.
Set the Decimal Places drop-down to 2.
Click Settings to display the Settings dialog.
Step 9
Display the Text > Dimension Text sheet, ensure Apply to Entire Dimension is active then click the Color icon in the Format pane to display the Object Color dialog.
Step 10
Select Black then click OK to return to the Settings dialog.
Close the Settings dialog.
Step 11
Left mouse click the Arrow Line access handle to display the Arrow Line toolbar.
Step 12
Set the Arrow Type drop-down to Closed Solid Arrow.
Step 13
Click Arrow Line Settings to display the Settings dialog.
Step 14
Display the Line/Arrow > Arrowhead sheet and in the Scope pane, ensure the Apply to Entire Dimension is active then click the Color icon in the Dimension Side 1 pane to display the Color dialog. Select Black then click OK to return to the Settings dialog. Select Close the Settings dialog.
Step 15
Click to place the dimension.
If you aren’t able to place the dimension, check to make sure the Specify Location selection step is selected.
Step 16
Display the MBD Navigator. The PMI node appears when the first PMI feature is created in a model.
You can edit or re-open any dimension by either double-clicking on the dimension itself or double-clicking the dimension in one of the nodes in which it appears.
You can also right-click the dimension in a node and select Edit in the pop-up menu.
Step 17
Using the Hole and Thread Callout command. New in NX 1926.
Make the Top view the (Work) view.
Select Home Tab > Dimension Group > Hole and Thread Callout
Type: Linear.
Feature: Select the M6 Socket Head, 4762 Screw Clearance Hole Feature.
Step 18
Indicate orientation and location with the cursor.
Select Close.
Step 19
Make any final positioning upon dimension creation.
Step 20
Using the same file from the previous step, make the Top view the (Work) view.
Select Home Tab > Dimension Group > Hole and Thread Callout
Type: Radial.
Feature: Select the M6 Socket Head, 4762 Screw Clearance Hole Feature.
Step 21
Indicate the preliminary position of the dimension.
Step 22
Locate the final position of the callout.
This is how you would create dimensions on a part with in NX PMI.
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