Cannot Remove Hidden Lines in Assembly Drawing (Creo 2.0)

[wjamieson]

I'm currently working on creating a drawing for an assembly. As you can see in drawing mode, I've selected "No Hidden" as the display style. However, the wire still shows through the sheath in drawing mode (refer to the red circle in the picture below.) I've also attached a picture of the assembly in 3D mode to give an idea of the geometry. As you can see, the clip completely surrounds the wire. How do I prevent the drawing from showing what is inside of the sheath? I am using Creo 2.0.

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[MartinHanak]

William,

what kind of geometry is created in your parts, solid or surface ? In case of surface geometry, you can set Hidden line removal for quils to Yes in Drawing View dialog box.

Martin Hanak

[dschenken]

There is probably interference between the two parts, which causes the software to be unable to determine which part blocks the other. Or, as Martin suggested, one or both parts are surfaces, aka quilts, which need to have the drawing mode to Hidden link removal for quilts set to be evaluated for hiding capability.

[wjamieson]

Thanks for the suggestions. I have changed "Hidden line removal for quilts" to "Yes" in the drawing view dialog box, as shown in attached picture. This did not correct the issue. Are there any other suggestions anyone might have? Thanks!

[MartinHanak]

William,

please upload the model and drawing, if you can.

Martin Hanak

[wjamieson]

Files are attached. Thanks for your help!

[Mahesh_Sharma · Accepted solution]

Wiliam,

Tried a quick test on file and issue seems to be due to accuracy of part wire__.prt. I set the relative accuracy of part wire__.prt to 0.001 and this corrected the view display.

[wjamieson]

Thank you. Could you explain where I go to in order to change the relative accuracy?

[Mahesh_Sharma]

Open Wire part, File > Prepare > Model properties > Accuracy Change > Set relative value as 0.0001 > Regenerate Model > Open drawing and that will be corrected.

[wjamieson]

Thanks so much for your help! The issue is resolved.

[dschenken]

Part accuracy affects the interference. Leaving it as Relative accuracy will allow the problem to return if the part size changes. It works by adding significantly to the geometry the computer has to process to get a smooth shape. Making the holes even slightly larger would avoid the problem as well, but without increasing the processing required and without the risk of the interference returning,

[wjamieson]

Also, by interference between the two parts, do you mean that the holes in the sheath might be too small for the wire, causing the material in the sheath to overlap the material in the wire? I drew the sheath in assembly mode and made the holes in the sheath the same diameter as the wire.

[dschenken]

The surfaces and the potential interference are based on the approximations by tesselation. They are not geometrically perfect. You might try measuring clearance between the parts, or just make the holes larger.