NX Hidden Edges Tolerance? Visualization changes with view scale in Modeling

[jmarkus]

Hi,

I've noticed that when I am using the static wireframe mode, with static hidden edges invisible (under visualization preferences), the accuracy of the hidden line view changes depending on what my view scale is. When I set my view scale as 1, it does a poor job and hides edges which should be visible. As the view scale is reduced (below 0.7) then the hidden line view appears correct (no missing edges). Is there another tolerance setting somewhere which is controlling this behaviour?

Note, the reason I am trying to get this to work is for exporting CGM files of various modeling views - which only exports as hidden line with the 'static wireframe' rendering mode (as opposed to the 'wireframe with hidden edges' rendering mode).

Thanks,
Jeff

 

[cowski]

For the static wireframe, you'll probably need to use view -> operation -> "regenerate work" after each view manipulation (scale, rotation, etc).

You mention exporting CGM files from model views. Have you considered creating a drafting view and exporting that instead of a model view? I've had pretty good results using that technique. Create a new drawing sheet (blank sheet, not a template), add your view (turn off view borders), and export to CGM.

www.nxjournaling.com

 

[jmarkus]

Cowski,

Using regenerate work doesn't change the behaviour. It regenerates 'correctly' for small view scales and incorrectly for larger view scales. Maybe whatever controls this tolerance is not accessible in the preferences...

I'll see if the workaround of making a drafting view first will help.

Thanks,
Jeff

 

[cowski]

If the part geometry is good and you can reproduce the issue, I'd suggest opening an incident report (IR) with Siemens support.
faq561-2116

www.nxjournaling.com

 

[jmarkus]

I tried a couple of different assemblies and it seems to only occur when the assembly has PMI, but not with all assemblies with PMI. I have opened an IR with Siemens to see what they say.

Thanks,
Jeff

 

[jmarkus]

I spoke with Siemens. It turns out there is a bug in how the Parasolid kernel handles hidden line removal when the assembly contains interfering solids. In a later release than I have (I am using 1973) they have added some additional settings to help manage this in the Static Wireframe rendering style preferences. As a work-around, you need to somehow eliminate the interfering solids - either boolean them with the surrounding solids as appropriate or simply blank them from the view. Note that the 'accuracy' of the hidden line removal (or lack thereof) is not necessarily compromised where the solids interfere, but can occur in an area of the solid seemingly unrelated to the interference, due to this bug.

Jeff

 

[cowski]

If it is a case of interference, the drafting views may be the way to go. In the drafting view preferences -> hidden lines, you can turn on the "process interfering solids" option and the "display interference curves" option. This might be easier/faster than fixing the solids.

www.nxjournaling.com

 

[jmarkus]

Cowski,

I did think about your suggestion of using drafting views. The problem I see is that I am trying to make 1:1 CGM images quickly from files with multiple model views - all of which have different extents/bounda (both among the model views and across the files). I had a journal which exported PDF images of the model views and I was modifying it to do the same for CGM images. I'm sure I could put together a different journal altogether that gathers the necessary information from the model views and creates a unique sheet size for each one, etc...and export the CGM file from there - but I decided it wasn't worth the effort. Now that I have come across this issue (which only applies in certain situations), I think I'll wait and see how often it becomes an issue.

I appreciate your help as always!
Thanks,
Jeff