Making Working with Someone else's NX Models Easier (maybe) 2

[alj722]

I am involved in developing a standard to simplify (hopefully) exchanging NX models with those outside our organization. The goal is to reduce confusion and rework by requiring our users and our contractors to follow a (small) set of best practices that address interoperability problems. An obvious example is requiring all users to use the same base units.

Those of you who have been through the pain of trying to work with another organization's model, what things have caused you the biggest problems? What things have you done that helped fix those problems? If you could contractually make your vendor model a certain way, what would you make them do?

Thanks for your help. Who knows, you may end up having to model to our standard someday - so suggest things you can live with.

Drew

 

[RUGmechanic]

In my experience:

1 Use the master model concept
2 Agree on naming (conventions)
3 Layer settings
3 NX version
4 Use of Colors to define / identify materials in modelling
5 Use Groups to logically group features / solids

"Biggest problems": What features to use to build a model.
Like block, 2 slots or sketch, extrude, sketch, 3 extrudes.



Older budweiser

 

[ewh]

I agree with many of the above, except I would not be as concerned about layer settings as that they be fully catagorized, and I feel that requiring certain colors to represent certain materials to be overkill. You will often find that people tend to choose colors to aid them in design, and I don't think it necessary to mandate colors as long as the pertinent properties are still identified is some manner. If you have an assemble of parts made of the same material, you just lost a design advantage you may have had by making them all the same color. Of course, I still often see organizations that try to control these type of issues to the Nth degree (specific colors for every type of drawing entity for example, even though the part will be made to a monochrome drawing), but I see little value added in micro-managing such properties. Effort would be better spent in other areas.
Remember, you are dealing with another organization, and you should give them as much leeway as possible as to how their procedures are written as long as they interface with yours with as few problems as possible.
As to the modeling side, it is often still the wild west ;-), and the same advice applies as long as the file can be easily disected. There are so many legitimate methods to use in NX, it would entail more effort than it is worth to dictate that only specific methods be used, unless of course it will effect downstream processes.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[johnnyalexandr22]

first of all go to
-customer defaults
-general
-manage current setings,
-make an export defaults

then you can give the file with the default to anyone that you want to have the same defaults with you. The only think that he must do its an import defaults

 

[alj722]

Very helpful - Thank you everyone.

Drew

 

[alj722]

johnnyalexandr22 - what version of NX are you using. I can't find an export option for the defaults in NX7.5.2

 

[alj722]

johnnyalexandr22 - Never mind. Found it.

Thanks

Drew

 

[cadmantools]

Modeling and cad standards are good for consistency and helpful when changes are made by various personnel and not the individual which originally created the part over it life cycle. The pain is in enforcing these procedures. It helps a lot to write application software to help maintain and automate the process. This will speed up the design process and by reducing the checking requirements and will encourage the procedures to be followed.

NX6.0.5.3 mp07, Windows XP 64-bit,Team Center 8.1
Running cad straight out of the box is OK but, a system tuned with application software is the best way to increase productivity.

 

[ewh]

Just don't go overboard...
I just completed a CheckMate run that took over 8 hours, having to run overnight, just to catch incorrect section arrowheads, section view text height (which was correct, just not defined the way CheckMate was checking for), and many other non-value added things.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[edgray]

I propose standard principles not specific standards.

Have a standard layering system.
Name the layers. Long descrptive names.

Name all sketches in a way that removes the name "sketch" tha comes after the feature number. Long descrptive names.

Name features to label the beginning and or ending of graoups of features the form a "feature" of the part

I am not decided on the utility of groups. They can obscure things if done sloppily.

I council not to use the simple features hole, block etc. My feeling is that they are too constraining. i prefer to sketch a circle and extrude it. Later if I want the hole to be square or octagonal no problem. With the hole no chance to change and all the features that depend on it will have trouble when you delete .it

Don't sketch on a face. Create a datum plane in the location maybe even offset 0 from the face. This just simplifies the fix when the face dissapears.

Use experssions whenever possible. It enhances the "what if" experiments.

Think in terms of change. don't add a feature if you can do the same thing by adding or subtracting curves from a sketch. The less feature the better!!!

Think in terms of change.
How might this dimension change in the future?
How might this feature change in the future?
How might this part feature change in the future?
etc.

My experience is in very large parts >3000 features but following these guides my parts are very adjustable.

Good luck!