In NX drafting I am getting incorrect dimensions. It happens when users pick a model edge which has some "garbage" entities so the resulting dimension in incorrect. However, the bad entities can be seen only when zooming in quite close. Measurement of the solid model in the modeling application is not showing any sort of edges hanging down below the bottom face. I am not sure if there are settings to address this but I have looked through docs and customer defaults for hints as to what is going on and have no solutions so far.
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As far as I understand, you don't know where these garbage entities, come from. I have never seen something like that, but I have some ideas to try:
1. In the view settings, set the tolerance to zero. After regenerating the view, the tolerance is re-calculated (auto-adjusted). Just a guess but probably doesn't work.
2. Examine Geometry. Maybe the geometry is corrupt and drafting can't deal with it properly.
3. Try to find out what object types you are dealing with. Like Information -> Object
4. if none of it works, probably GTAC can help here.
That helped, thank you! I will keep an eye on it for a while and hopefully this is a long term fix.
By the way I looked in customer defaults for the view tolerance but cannot locate it so is this set in File-Preferences-Drafting-View-Common-Config?
Are you dealing with imported geometry? If so, you might try the "heal geometry" and/or the "optimize face" commands; they can help clean up small geometry errors.
No, it is native NX geometry. The bottom of the model, where the image is taken, is flat with some prismatic features in the bottom face, CB's, slots, etc-.
I use heal once in a while although haven't tried it for this issue. I will give it a try.
I'm still trying to find the customer default setting for the view tolerance.
If it is native geometry, I wouldn't recommend heal geometry as it will remove the model parameters. Start with "examine geometry" to see if it turns up any model errors.
For the customer default option, try drafting -> view -> general -> tolerance; I believe that is the same tolerance mentioned above. Bear in mind that the setting is part specific, so you will need to change the setting in your drawing template to affect new drawings.
Healing does not present many problems for me. Sometimes we have to heal when the part from the end customer is dirty or the the internal native part becomes dirty from numerous complex 3D intersections resulting from design constraints.
Also it is not uncommon for manufacturing eng to work from dumb models because often we receive files from customers which are step or parasolid.
I am not seeing drafting -> view -> general -> tolerance in customer defaults. Are you on a different version than I?
Sorry, that was for the NX 9 location. In NX 10 it seems you need to customize the drafting standard for some odd reason. Customer defaults -> drafting -> general/setup -> standard -> customize standard -> view -> common -> configuration -> tolerance.
To change the part setting, go to: Preferences -> drafting -> view -> common -> configuration -> tolerance.
Thank you. Wow, I completely spaced out where that was. It has been a long time since I customized my drafting standard. Well I checked it and it it is set to zero so I am not sure where it is picking up a tolerance from.
Although, and please humor me for a minute, I believe there are some file-preferences which are global and not merely per session. I have gone the route of new part files defaults using blank so this may be where some of my issues are from. After setting File-preferences for the tolerance then restarting NX, new files seem to be using the new tolerance.
"Well I checked it and it it is set to zero so I am not sure where it is picking up a tolerance from."
NX can't actually use a value of zero for the tolerance; it is just a special value that tells NX to "calculate a tolerance for me and use that". Once the tolerance is calculated, it is saved with the view. As your model changes, the tolerance value may not be the one that works the best; that's when it is time to supply a new value (or enter zero to recalculate a tolerance).