Edit dimension in Drafting -> changes model? 4

[peterrdevries]

Working Master Model Drawing.
Is there a way when to change a Drawing Dimension and automatically the expression of the 3D Model is also changed?
Or with other words, toc change my model in the drawing.

Thanks in Advance, Peter

 

[braddles90]

Nope, that functionality doesn't exist. I think it's driven by the 'master model' approach - the model drive all downstream data, so I think it works against that to have the downstream files change the model.

I *guess* you could, however, have an interpart expression link between the drawing file and the model file, but then I'm pretty sure that you'd only be able to change the expression in the drawing file - there's no way to have both files able to modify the dimensions on the part.

Hopefully someone else might be able to explain that a bit better :

 

[cubalibre000]

Yes, can be done if you have PMI license and convert dimensions that you want to put in the drawing as PMI.
Then import PMI diemsnion from part
You must enable this functionality in the customer default.

Thank you...

Using NX 8 and PDM RuleDesigner

 

[Xwheelguy]

There is also another method that involves inheriting the sketch dimensions. For this to work, you have to sketch, add sketches to specific reference set (at least you used to have to do this), then the sketch dimensions will show on the face of the dwg and you can edit them there, which will drive a change to the model. Take care in how you set up diameters in your sketches if you use this method.

Check out the NX documentation for "Inherit Sketch Dimension" in the Drafting section.

I'd also suggest including the version of NX you're using whenever you post a question, as it helps us help you if we know that information up front.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[braddles90]

Whelp, I stand corrected...

I was thinking of (I think Inventor or Solidworks?) where I think this is a standard function for all parts, rather than seemingly having to set it up for each part you want to do this with as described above.

 

[CAD2015]

Xwheelguy,
I tried to follow your advice, but it doesn't work!

MZ7DYJ

 

[Xwheelguy]

braddles,

You don't necessarily have to set it up for each part. You could use templates or start parts to accomplish getting the reference sets prepared - that's about all that is specifically required other than how one chooses to model the part (sketch or no sketch), in which case a sketch is required for this workflow.

Personally, I've not found a good reason to use this, as you have to really think ahead when sketching for it to work flawlessly in every situation for every part you're going to create.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[CAD2015]

Cubalibre00,
I try to use your suggestion:

"Yes, can be done if you have PMI license and convert dimensions that you want to put in the drawing as PMI.
Then import PMI dimensions from part You must enable this functionality in the customer default. "

I have two questions:
1) How should we convert dimensions that we want to put in the drawing as PMI?
2) How should we import PMI dimensions from part?
Can you present us a step-by-step complete procedure?

Thanks!


MZ7DYJ

 

[JohnRBaker]

Actually there's a Customer Default which controls whether Expression are available to be edited while in a Drawing and I suspect that the vast majority of our customers have turned this option OFF, and in some cases, have probably gone out of their way to LOCK it as such, as this is considered to be a very poor practice at best. In fact I can recall how when we first announced that this capability was being added to Unigraphics (this pre-NX) that our largest two customers are the time demanded that if we did do this that thered needed to be a way that it could be disabled as they would NEVER allow something like that in their offices. With the current state of the art for CAD/CAE/CAM/PDM systems it is standard practice that the Models, NOT the Drawings, are where the 'math' or part data-model exists. Drawings are simply a 'document' showing what is to be manufactured, but they are not being used to actually manufacture the final product.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[peterrdevries]

John,

Can you please add the Customer Default (NX9), to test.

Thanks in advance.

 

[looslib]

I have heard of horror stories of users of another CAD product that has this capability on by defasult and the amount of scrap it has produced. One item was a V10 engine block that the drafting guy changed a dimension and then manufacturing took the model and created NC cutter paths. The block was scrapped when they discovered the drawing change. This company had been a UGII customer, went to this new software for its parametric approach and has since switched their manufacturing plants back to NX.

Chinese proverb: "Be careful what you ask for."


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[joycejo]

I agree with Ben. This is IMHO just a disaster waiting to happen. If you need the environmental variable contact gtac. Please don’t post it in a public forum. Change the model to drive the drawing not the other way around.


John Joyce
N.C. Programming Supervisor
Barnes Aerospace, Windsor CT
NX6, NX7.5,NX8.5, NX9.0
Vericut7.3

 

[ewh]

What may seem a shortcut to get the dimension you want on a drawing may affect many other parts, depending on assembly size. It is always safer to do as mentioned above and let the model drive the drawing. Otherwise you may end up with some unfortunate unintended consequences.
Now, in the rare situation where this is a single, stand alone part that is not (yet) used in any other assembly, you may get away with it (but it would still be poor practice).

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[peterrdevries]

Thanks for all your comments.
Peter