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Purple Hidden Lines appear in "No Hidden Line" Dra

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Newbie

Purple Hidden Lines appear in "No Hidden Line" Dra

I have imported in my project several parts and assemblies from different manufacturers, both in Pro/E native files and .step formats. Some of these exhibit strange line behavior in drawings. While my drawing view is set to "no hidden", some parts still show up with hidden lines and are purple in color. Any ideas what could be causing this?
7 REPLIES 7
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Purple Lines

The purple objects may be independent surface features, as opposed to "real" hidden-line representations of solid features. Check the model tree if it's a native Pro/E file.
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RE: Purple Lines

Did you set the Hidden line removal for quilts to yes (in the drawing view properties>View Display)?
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RE: Purple Lines

hi, Andri Ulrich First you just check as per David,Sylvain suggestion. If still problem not solve then there are tw solution, 1)you can erase those lines what dont want... View>drawing display>edge display>erase lines.. select lines and erase.. 2)select that perticular view then layer properties >select layers >surface or curves hide...
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RE: Purple Lines

Thanks guys, setting the Hidden line removal for quilts to yes seemed to work....Too bad the lines are still purple, since I don't have any layers to work with I'll have to live with it.
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RE: Purple Lines

If you want them to have another color, just change the Quilt color in View>Display settings>System colors
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RE: Purple Lines

Did you try to select the imported quilt surface (you can use proe selection filter)and then Edit/ Solidify in order to create a solid volume from your imported data. then the external surface color should change form purple to white. After that you will be able to create a X-section across the assembly. X-section do not work with quilts surface. Good luck.
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Re: Purple Hidden Lines appear in "No Hidden Line" Dra

I find that most of the components I download STEP files for with threaded surfaces cause this issue. The small surfaces in the model are being ignored, either in the import or by the vendor's export features.

It's possible to correct the part, i.e. "Edit Definition" select the Medical Symbol " Enter IDD editing Environment", and then use the tools CREO provides to extend and trim, create, etc. The tools, however, aren't diverse enough to truly correct a part.

In those cases, I generally would tell you to either create the model solid, using the STEP import surfaces as references (or not) and then hide the original geometry (or delete/suppress) OR just move on and live with it.

Examples that cause this: Threaded couplers, pipe fittings etc. They woudl import as a solid were the threads not physically modeled. McMaster's CAD files provided by their vendors commonly do this. 

Examples that don't have this problem: SMC's air fittings typically do not model actual threads, but only show the cylinder that would be threaded. So these files import as solids.  

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