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Improve drafting in NX CAD, part 2: responsive drawings


This NX drafting-related tutorial shows you how to improve the of reusability of the drawings. It means that minimum efforts are required after a model is updated.

If you take your time to make a parametric model for reuse, you also should consider spending some time for making responsive drawing.


NX drafting tips and tricks.

The recommendations I show here do not remove the necessity to check the drawing after an update is done. However, they can guarantee that dimensions would be always be correct and overall minimum adjustment is needed.


1. Position the views in the responsive manner.

In case your model changes one of the main dimensions, your views could intersect with each other after update. Test the views with maximum and minimum size values (consider doing it when you start modeling, since update time is faster).

In case you require using View Break, define it from model elements (points, curves) and use an offset. Make sure the points are defined associatively.

NX draftingCreating View Break, positioned associatively to view elements


2. Try avoiding the situations when dimensions can lose associativity or have incorrect value.

NOTE: From my experience these happens with about 5% of dimensions, primarily on the complex assembly drawings. You may not need to follow these recommendations if you don't notice similar behavior. Please, add your comments if you can identify the reasons for dimensions losing associativity or have incorrect value.

I have noticed two major scenarios when above-mentioned problems appear. There are ways of putting these dimensions so that that value would always be correct (described in part 3)

Check carefully the following dimensions:

  • Dimension is attached to a feature, which renews its surfaces after update (for example tube feature with multiple segments)
  • Dimension put onto geometry on break-out section (inside break-out section or from break-out section to normal line)
NX drafting
Dimensions taken from break-out-section can cause errors


3. Make sure that the dimension value is always correct

NOTE: These technique can only be used if there is a risk of a problem with dimension (described in part 2).  Normally you create dimensions as shown in NX training. If the problem repeats frequently consider implementation of PMI in your department.

To make sure that value is always correct, you can take the dimension value directly from a sketch. To do so:

  • Decide about existing, or create a new sketch (it is also possible to use sketches, that only have reference dimensions)
NX drafting
Both dimensions from this sketch will be extracted
  • Use Feature Parameters operation to extract the sketches into drawing
NX drafting
Normal and reference dimensions are extracted onto a drawing


Second possibility is to connect the value of expression directly:

  • Create a dimension (value would be changed later to correct one)
NX drafting
Dimension, the value would be changed to value of expression
  • Right-click on the dimension
  • Choose Edit Appended Text
  • Click on the dimension value and remove it in Text Editor dialog
  • Then go to Relationships, Expression
NX drafting
Value is removed from dimension, location for linking an expression is shown
  • Navigate to the required expression (you can select one in the assembly components or top assembly part)
  • When done with selection fix the amount of decimals (by default is set to two)

NX drafting

  • When done, edit the dimension style

NX drafting

4. Make sketch views updatable.

When you need creating a sketch-based view, you can also make it updatable.

  • Create an empty view (By using Insert, View, Drawing)
  • Start Active Sketch View and draw a sketch


  • Add the required dimension to sketch and make sure it is a Driving Dimension
  • Then edit the dimension value using Formula
NX drafting
Way to link an expression to the dimension


  • Navigate to required expression, if needed use interpart expression
  • The dimension would now guide the sketch similar to modeling

5. Use expression-based annotation suppression.

  • Make sure expressions are allowed in drafting: Customer defaults, Drafting, Drawing, General, Allow Expressions. 
  • Create an expression (with value 1 for shown or 0 for hidden)
  • Choose Edit, Suppress Drafting Object
  • Enter the expression name and choose object to be hidden

6. Use associative positioning for drafting objects.

NX drafting
Correct way to position detailed view

Some drafting features (for example detailed views, view breaks, section lines) can be positioned with relations to view objects (curves, points) on a view. When you position the features in this manner, they will become associatively connected.




The use of above-mentioned techniques can reduce the time for adjusting a drawing to new dimensions, it can also reduce a possibility of making a mistake. However, it takes time to define all the relations.

Have you encountered problems with updatable drawings?


About the Author

Alexander Popkov is the NX CAD/CAM method professional, currently working in Industrial Machinery.

Along with Maxim Semenenko, he runs a blog dedicated to the medium and advanced NX CAD/CAM tips.