Model dimensions in drawing 2

[JModelsalot]

Hello anyone/everyone, I am a new NX user coming from PROE, Solidworks, Autodesk 360 and OnShape. Modeling is modeling with each of these in their own way but I can not for the life of me figure out how to parametrically link all of the model dimensions to a drawing with NX.

Is there a way to keep all of the dimensions linked so that a person could change info on the drawing to change the model (if they felt inclined to do so)? As far as I can tell I am expected to add dimensions on the drawing and they are essentially reference dimensions as they have no real value to the math model.

I have read info from another forum that was closed years ago but there was no solution found then and I'm hoping something has changed 6 years later.

If there is not a fully developed solution for this please say so as this functionality is too basic to need a work around. If NX cant fully handle this thats fine (although terrible) and if nothing else I can stop playing elite level Wheres Waldo!

 

[JohnRBaker]

Have you had any formal training for NX? If not, I would recommend that you look into getting something going, either in a classroom or online.

John R. Baker, P.E. (ret)
EX-'Product Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[jerry1423]

NX works pretty much like the other CAD system. When the model is changed, the dimensions on the drawing changes too.
What do you mean by PARAMETRICALLY LINK ?
You will find basic training like this on YouTube.
If you are looking to change your model dimensions from the drawing, that is available too

https://www.eng-tips.com/viewthread.cfm?qid=385712

Jerry J.
UGV5-NX1961

 

[JModelsalot]

@John Baker,

Thank you for the info but I was really hoping to know if its possible to do what I'm asking in a non work around manner. What I'm asking is as simple as the extrude feature on other platforms so youre answer leads me to believe thats a no. If so that is fine, I have come to expect it at this point.

That being what it is, if I were to get specialized training for basic functionality, would there be a specific bit of training that I should be sure is part of the curriculum?

 

[cowski]

For sketch dimensions, you can use the option "display as PMI", then inherit those onto the drawing view.

...a person could change info on the drawing to change the model...

In general, no. There is an option buried somewhere that allows you to edit modeling expressions in the drafting module, but even with that turned on, your editing of the model will be limited. To make meaningful model edits, you really need to be in the modeling application. To the best of my current knowledge, you cannot double click on a dimension on the drawing sheet, edit the value, and update the model.

www.nxjournaling.com

 

[JModelsalot]

@Jerry,

Thank you for the reply and thinking about my question but when I say parametrically link I mean the model, the drawing and its dimensions are one in the same. I agree, NX works pretty much the same as other software minus a great deal of inferred intelligence, but it is what it is. In some platforms when you make the model, you can very easily pull the dimensions in the model to the drawing. Not a new dimension to look like the models, the exact parametric expression. Later, if you want to edit simple features you can change the dimension in the drawing and it will update back to the model. Therefore, parametrically linked, not a copy, the same exact thing.

The link you sent is where I started as I was searching for the PTC/Creo functionality that the thread creator had mentioned. He was unable to find much other than a disjointed work around as well.


@Cowski,

Thank you for your reply as it is what I expected and it is the answer I was looking for but not hoping for. You mention a work around but thats not worth the effort to get something that someone down the line may not be able to understand when making changes to the data.

Thanks for the info everyone, you saved me a fair amount of searching for something that is not intended software functionality.

 

[Ehaviv]

I think the future is no dimensioning
at all.

 

[JohnRBaker]

...you saved me a fair amount of searching for something that is not intended software functionality.

How does one go about searching for something that is not there? ;-)

John R. Baker, P.E. (ret)
EX-'Product Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[cowski]

How does one go about searching for something that is not there?

Are you trolling, or is this just a dumb comment?

www.nxjournaling.com

 

[JohnRBaker]

I was trying to be sarcastic (see the smiley face). It just seemed like a odd thing to say.

John R. Baker, P.E. (ret)
EX-'Product Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[Crocostimpy]

I think people are misinterpreting the question. What the OP is talking about is showing the actual dimensions from the features in the model on the drawing so that one can edit those dims and the model will update without having to open it separately. And yes I know that the model will open in the background anyway when opening the drawing.

Many years ago I used ProE in a previous life designing plastic packaging. I would purposely include dimensions in my sketches or whatever that I would then show on the views in the drawing. It could be a little bit of a timesaver to modify the model from the drawing, provided nothing blew up during regeneration that is.

I have never found a way to do that in NX.

Mike

 

[JohnRBaker]

Part of that is based on the philosophy that the model is the definition of the part, NOT the Drawing. I realize that this is an evolving concept, but that's the way things are headed.

John R. Baker, P.E. (ret)
EX-'Product Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[TheTick]

Is there a way to keep all of the dimensions linked so that a person could change info on the drawing to change the model

Editorial comment--I find this a loathsome practice that often leads to more harm than good. (p.s. Regardless of which CAD platform.)

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[JohnRBaker]

In fact, we had several large customers, particularly in the aerospace and automotive sectors, who told us when they were evaluating our systems, that IF we DID offer a mechanism whereby the person creating/editing a Drawing could change the dimensions of the part Model from the Drawing, that we would have to provide a scheme by which this capability could be permanently disabled.

John R. Baker, P.E. (ret)
EX-'Product Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[looslib]

I remember hearing of a story that a drafter changed a couple of dimensions in a drawing that caused the model to update and thus the NC program, too. Scrapped a few parts. This was not UG, but Pro/E and the parts scrapped where not cheap! Think V12 engine block castings.

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

Ben Loosli

 

[3DDave]

The "all drawing dimensions are created" space is usually touted because the model makers have no idea how they expect their dimensioning, which drives the model, to drive the model. To copy from the movie industry, they "fix it in post." I call it "planning after."

This ends up with the model scheme and the drawing scheme able to diverge. It often means that what looks like a trivial change on the drawing is a massive change to the model with unexpected interactions - the very sort of interactions that are worried most about.

But here's a secret - it supports a make-work industry between engineering and drafting. I came across a contract drafter who built a model from an existing drawing with model dimensions linked 5-10 deep so that changing a wall thickness required changing all those other dimensions to make a drafting dimension change per the Engineering Change Request. Similarly, for years our CAD drawings weren't allowed to have trimetric views. Why? Because the head of manufacturing had a buddy who was great at making trimetric views by hand with AutoCAD - his only talent - for process instructions and if engineering put them on the drawings, that guy would lose his only job. I sneaked one into a drawing for an engineering prototype (no manufacturing management sign-off required) and the welders were like - "Can this be on every drawing?" Nope. A lot of people had to pass away or retire to let that happen.

If they don't want the drafter to be able to change the model - release the model and lock it against changes. It's that simple.

Did the major customers also have a plan to require that all required dimensions were on the drawing, that no duplicated or double-dimension schemes were there and that no dimensions were simply sketched from lines and drawn with drafter supplied text that isn't an actual dimension? I ask because I've seen the "fix it in post" drafters do all of those things, including creating a faked BOM because they didn't know how to change the assembly to use the required parts. Sure the model shows a .5 inch long bolt that clears mating parts, but the fat-fingering of the fake BOM called out the 1.5 inch long bolt.

If the CNC program changed, then that is what the drawing change was supposed to do. If it wasn't, those should have been caught by the checkers. More than that - the CNC programs should be controlled the same as any other data. If a particular release of the model is going to manufacturing then manufacturing should only use that version of the model and not go with "latest." That's stupidly careless otherwise. Better to blame software than poor management.

 

[JModelsalot]

Dave,

After working with several previous software's and now moving to the NX sphere I have to agree with your initial statement about how models are created. I seldom open models that do not have additional features added rather than redefining previous ones appropriately. Its second nature at this point to plan the sketches and features in a way that can be used downstream. There are caveats to this with expressions and feature relations but for the most part a model could be set up and dimensioned in a way directly usable downstream. It may not work in all instances, but its better than creating model intent and dimensions 2x and doing it at a level that is expected to be supportive(the drawing) to the math model.

Interesting posts about why this practice is not common as much of it included things I had not previously considered.