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NX 10 and Bidirectional editing

Valued Contributor
Valued Contributor

Hi all, I have some questions on NX's ability to do bi-directional editing.


Here are the scenarios:


1) In a drawing, is it possible to create dimensions that drive the model and/or a Part Family spreadsheet? So, create a dimension that is editable. I see that you can "allow expressions" in the customer defaults and I can see that you can create a rapid dimension that is "driving", but I can't get any of it to work. Please post a workflow for this.


2) Model updating a Part Family spreadsheet. If I have a part, is it possible to change a sketch dimension that will update the spreadsheet? Or once you apply dimensions in the part family spreadsheet, it is only 1 way directional?


Thanks, Peter


Re: NX 10 and Bidirectional editing

Siemens Phenom Siemens Phenom
Siemens Phenom

For #1, the Customer Default, "Allow Expressions", simply means that NX will allow access to the expressions found in the Drawing file WHILE in the Drafting module.  This is really only useful when you're NOT working in the 'Master Model' mode.  Besides, it's basically an old concept that most people would just as soon not be reminded that it's even possible.  In fact, when we first proposed doing this, it was primary so that we could 'demo' this capability when we were in competitive situations, but many of our larger customers demanded that they be able to turn this capability OFF, thus the Customer Default setting.  Personally, I would leave it turned OFF and pretend that it just doesn't exist.  In the end, you'll never miss it.


As for #2, if you're talking about a Part Family spreadsheet, the answer is NO, you can modify the content of an existing spreadsheet by edit an expression in the part file.  Spreadsheets inside of NX just don't work like this.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA

Re: NX 10 and Bidirectional editing

Siemens Legend Siemens Legend
Siemens Legend

Just my 2 cents to #1:

There is a way to bidirectionally edit Model Parameters, even when working in Master Model Mode (drawing part references model part): The editable dimensions must be PMI's, that are based on feature dimensions.


Prerequisite: There is a customer default that needs to be switched on:

Drafting -> General/Setup -> Workflow Tab -> PMI Edit section -> "Allow PMI Bidirectional Edits"


I uploaded a video that shows the general workflow.


Re: NX 10 and Bidirectional editing

Valued Contributor
Valued Contributor

Thanks guys! This definitley helps.


The way we are using the CAD package, we really need this functionality to produce a lot of 2D files quickly. PTC Creo really kicks NX here....bidirectional drawings and spreadsheets are standard there and very easy to work with. This is not to say NX is bad, just different with different strengths.


I hope Siemens can also clean up the Part Family spreadsheet functionality for release 11 or 23, as it is super clunky and slow.


Re: NX 10 and Bidirectional editing

Valued Contributor
Valued Contributor

Well, I might has spoken too fast.


The PMI seems to work and show on my drawing, but since the drawing view is showing an instance from the Part Family spreadsheet, I can't actually update the drawing dimensions to update the spreadsheet to update the part....too bad.  Creo wins!


Re: NX 10 and Bidirectional editing

That truly depends on your company and the roles of the people running your CAD. The last thing I want is to have a designer or draftsperson making changes to the models while in detailing the part.
The same logic applies to Part Families. Your family table is defined and should be read only. I don't want people making non-standard sizes of parts that could; 1) significantly increase the cost of the assy- due to custom part. 2) making tweaks to standard parts to fit a single design. 3) adding members to family that aren't approved.
If you are in a managed environment then you need to think about the versions and revision too. It just opens up to many Pandora Boxes!
Now you mentioned you need to create 2D elements. I'm sure there are plenty of tools to allow this that can be "programmed" or have rules written to control/limit shape and size as you add the symbol / sketch, etc to your part/assy.