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Hello Guys,

                      I have a query in NX Drafting,

                      is there any option in nx to hide Feature detail.

                      I Used the suppress feature but after supress, next dependable feature also disabled.


For Example:- I attached a pulley drawing image, in this i wanna Hide Feature & get Multiple Front View in Drafting for detail dimension,


1. With Pulley Teeth

2.Without Pulley Teeth 

Because i have to hide Pulley teeths , so i can see the detail like slot , hole etc.


So How to get two view with & Without Teeth In Drafting.......Pulley_7.JPG




Warm Regards
Thomas Roman
Machine Designer

Re: Hide_Feature_In_Drafting_View

Honored Contributor
Honored Contributor

You could try view dependant edit, but that would be abit labor intensive.  Personally, I'd look at sections, or other views, to show the details you need.

NX1867(if it had versions) | Teamcenter 11.6 | Windows 10

Re: Hide_Feature_In_Drafting_View

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

If the teeth were added last to the model, here is an option:

  1. In the model file, roll back the feature history to the point before the teeth were added.
  2. Use the "extract body" command (with the 'at timestamp' option turned on) to create a copy of the pulley at that stage of the model (no teeth).
  3. Remove the 'no teeth' solid from the model reference set and create a new reference set for the 'no teeth' solid.
  4. Add the model to your drawing file using the 'no teeth' reference set.
  5. Add the views of the pulley with no teeth.
  6. Use "hide component in view", "layers visible in view", or "view dependent edit" to hide the model that you don't want to see in the view.


Re: Hide_Feature_In_Drafting_View

Siemens Esteemed Contributor Siemens Esteemed Contributor
Siemens Esteemed Contributor

Another suggestion would be a breakout section view - though probably not suitable for your application.

Take a look at the attached - I've assumed that your drawing is in the same part as the model.  Sheet 1 show's Dave's suggestion - a simple section view - which gives you everything you should need.  Cowski assumed your drawing was in a separate part, however, you can use a similar method if the drawing is in the same part (and you can eliminate Reference Sets).  Use the Extract command to extract a copy of the body prior to the teeth being created.  In the attached part I placed the Extracted Body(8) on layer 10 and used "Layer Visible in View" to hide everything except layer 10 for the views on Sheet 2.  I also made layer 10 'invisible in view' to hide the Extracted Body in the views on the other two sheets.  Sheet 3 shows how you could use Break-out section to look inside the part.


If this was a featureless (unparameterized) part you could use a similar principle to the Extract Body solution except in reverse - extract the body and then use synchronous modeling commands to remove the teeth - such as Replace Face.  Place the extracted body on a separate layer and use Layer Visible in View.  It seems like a good enhancement to have in NX - the ability to add a view, with an option to show it up to a specific model history timestamp.  ER 6259252 already exists in our system asking for the ability to suppress features in a view on a drawing sheet.


Regards, Ben

Ben Broad | PLM Enthusiast | Siemens GCSS

NX (v17 - 1876) | Teamcenter (9 - 12)
Value Based Licensing | Adaptive UI | BETA Registration

Re: Hide_Feature_In_Drafting_View


Thanks Guys


                      Thanks for support , I got the solution....

Warm Regards
Thomas Roman
Machine Designer