This needs to be set in your ugii_env.dat file, so that it is consistent with Teamcenter integration and Native NX.

The Template folder for Native and Teamcenter looks for a .pax file.

For Teamcenter pax files: (start with nxdm)

• nxdm_ugs_drawing_templates.pax
• nxdm_ugs_model_templates.pax

For Native pax files:

• ugs_drawing_templates.pax
• ugs_model_templates.pax

Within each of these pax files points to the name, and location of the files to be used. The Teamcenter files are pointed to Teamcenter Item/IDs with the syntax of @DB\ITEM_ID\REV

Set a variable: UGII_ENV_FILE=<location>\ugii_env.dat to have all your clients using the same configuration. Put this <location> on a share on a server, each seat would have this location mapped as a drive and one variable set to point to this location. Now you have complete control for all seats in your environment.

I’ve decided to write about this because of a hair pulling discussion I heard the other day about two people debating whether to use parametric modeling techniques or edit the solid model at the parasolid level. The debate/argument went like all the others have. It went something like this: (person 1) I can make, create, edit faster using a parametric model. (person b) I can do it faster then anyone by editing the face. (person 1) without all those quick shortcuts and scripts? (person b) without anything, It is faster then using parametrics…. It seemed like it went on like this for ever.

Here is my stand point. There may be some people out there that can edit the faces of the solid and do it faster then someone editing parametrics. I doubt it but to shut them up for the moment we will agree. But the time they save, sacrifices down stream users. Some history about NX, All faces have an internal ID, when you create a mating condition, analysis, drawing, assembly, anything, NX uses this ID to keep track of what is going on. When you edit the faces, offset, remove and add blends, etc. That ID changes. So you saved 3 minutes on this solid but you cost more work for everyone else. Because now those face ID’s are different and the dimensions need to be reassociated, new mating conditions, edit the mesh on the analysis. So the big picture you caused more un-needed work. I hear the debate for mating conditions from someone already… What if we don’t use mating conditions, or if we do use mating conditions they complain that NX should update based on some black magic voodoo. Well the best thing that could happen is if there was an issue the part used in every assembly moved drastically for everyone to know. But most likely is that it could have moved ever so slightly that no-one will know exactly what moved, how much it moved, or why. Causing even more work.

Lets forget about the downstream users for a minute (like most people do). The debate about speed in the current model is still on. The way we look at it is, every part should be setup in a way that makes it easy, quick, and precise way to edit it. Give the part of the unparametric solid to someone else and they will be so frustrated, hacking it up, and waisting time. The cocky person that made this crap solid is probably saying, “It’s easy, why don’t you know how to edit it, you are dumb” well something like that. This is a classic result of job preservation attitude. No matter how stupid that is, people feel that if I make it so easy to edit it, i’ll be out of work. Again, they are looking at the big picture. The company your working at is probably turning away work or sending it elsewhere because they need it done and everyone is busy. You hardly ever see this directly because this is a management decision and all you see is the work in front of you.

Parametric models are your friends. Keep it Simple and easy for everyone to edit it. Add in engineering rules to determine the offsets, sizes, of your model. Refactor the solid as you go to extract difficult logic with simplier ones. Build an easy to use interface with clear names, why try to brag that you know more acronyms they someone else. side note: I knew of a company where the people actually made up acronyms in their own group that the rest of the company didn’t use, talk about dense). My last statement is, If we let the person take the prize on the quickest way to edit a solid is unparametric, how would they stack up on the second edit, third, forth. With parametric models this would be very easy to edit a second time, and so on. They would be able to make variants of the same model very quickly, updating the drawing, update the assembly, update the anaylsis, before the first person ever got done with the second model change.

If your thinking about flexible assembly components, parameters are the only way.

If you do have to import a solid from a supplier, or someone trying to preserve their intelectual property or reverse engineering a part. There is a great set of tools available, that allows you to take an unparametric solid and make it into an editable feature. That is called “Direct Modeling”.

Last statement, I have been hired to go to a company and automate building the companies parts. I’ve gone from extremes of full part automation (the users that felt they had to preserve their idea of job security repelled it like oil and water), even though the company was turning away work because they couldn’t get it done fast enough. The other side to fully automation, was to automate pieces of the work. Then combining them into larger and larger projects. The result was the company had more work, they need to hire more people to keep up with the work, and no one lost their jobs. Unfortunately the company that had the job security people making unparametric solids hasn’t laid off them yet. But it will happen, unless they change.

Regardless if your using NX3 or NX2 start getting used to the selection toolbar. Why? you may ask, because the selection toolbar is being further extended in each version of NX, and the class selection dialog is a old dialog that has been with us in the Unigraphics days since at least version 10 if I remember right. The interface of NX is moving towards a context sensitive type of interface and the old dialogs are becoming secondary windows if you can’t find the feature from the new floating dialog styles. So that makes me think that the class selection dialog is going to disapear in a upcoming release of NX. NX3 it is still here but NX4?, maybe. Everything you wanted to do in the class selection appears to be in the selection toolbar. You’ll need to be in Modeling for the selection toolbar to be available.

My advice is to get used to using this toolbar now. So to lower your transition when it is removed. This goes for some other dialogs also. That will be addressed in another post.

Working with Large Assemblies, Best Practices

REDUCE OVERHEAD

Load Options: Use "Partial Loading” NX can load components 3 different ways, Fully loaded, Partially loaded, with/with out wave data. Partial Loading loads enough information to show the part, but does not evaluate expression or interpart expressions Downside is if parts rely on other parts via interpart expressions and it has changed since last time it was fully loaded, you will not see the change. Making the part the work or displayed part causes NX to fully load the part

Load only Need Components: Large assemblies you may want to load no components and only turn on the necessary components as needed This may be a slow process picking and choosing the right component. For companies that deal with large assemblies and open them a lot it is more efficient to use "Design in Context". Design in Context is a Teamcenter Engineering application

Reference Sets: Use Reference sets to Display only the needed geometry. Usually reference sets only consist of solid geometry, occasionally it may contain wireframe to show a centerline or other similiar information Component

Filters/Sets: When working on specific assemblies for an extended period of time create a Component Filter so that you can quickly return to the previous configuration

Faceted Bodies: Loading a component with a specific reference set that is only a faceted body will lower the resources needed to start NX Faceted bodies consist of the outer skin of the body and approximations of the solid bod

INCREASE PERFORMANCE

Work Part Emphasis Assembly Preference: Making a component the work part, the system “grays-out” the non-work parts. To save on resources you can turning on Preferences -> Assemblies -> Emphasize. When enabled, the work part remains displayed in its current color, but the rest of the assembly is dimmed in the color specified in the color option.

Disable Smooth View Change: When switching between views, NX has eye candy to smoothly transition between views. This feature helps keep the user orientated to what view they are coming from and going to. The downside is that it requires more resources. In single parts and small assemblies this is not an issue but with large assemblies this may have a performance hit.

Backface Culling: Specifies whether the graphics driver should disable rendering of backfacing polygons in shaded views. When backface culling is enabled, any surface facets that have normals directed away from the viewer are not rendered. This reduction in the number of facets rendered can significantly improve graphics performance, especially on low-end and mid-range graphics devices. This should be enabled for large assemblies. Fixed

Frame Rate: Improve zoom, pan, and rotate by turning on Preferences -> Visual Performance -> Fixed Frame Rate. This will make Objects like components to be converted to cubes or hidden. Depending on the current zoom small features and components may be hidden or greatly simplified The lower the frames per second is best for performance.

Scene Reduction Method: If enabled, when rotating this will hide objects. When you stop the rotation NX will render the components correctly back to recognizable parts instead of cubes

View Frustum Culling: If enabled, Objects not displayed in the current view window will not be rendered