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K
kb-31-Visitor
1-Visitor
November 30, 2015
Question

In part module - Some of the features (say like ribs) should not to be sectioned (hatched), but the creo shows the hatching for the rib feature they are asking how to exclude that hatching . How to remove this?

  • November 30, 2015
  • 4 replies
  • 2634 views

P_20151128_185150.jpg


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4 replies

R
rubenvillarreal14-Alexandrite
14-Alexandrite
November 30, 2015

I'm not sure if you can do such thing. Maybe at the drawing level there are more options.

I would suggest you to create an incomplete rib after you already sectioned the part. Not quite helpful I know, but it is a solution.

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J
JonathanHodgson13-Aquamarine
13-Aquamarine
November 30, 2015

For representing gear teeth and splines, (similar issue), we include a thin cut where a tooth lies on the section plane.  For internal splines this is typically all I model, to keep the view 'clean' - no actual tooth representation.

Of course, you should structure your model tree so that you can easily suppress such features if you want to do FEA; and if you choose not to model gear teeth then the mass calculation will be less accurate.  But it's a good solution for drawings.

D
DonSenchuk12-Amethyst
12-Amethyst
December 1, 2015

Not possible unless you mess with the model. In that case both Ruben's and Jonathan's suggestions would work.

For Ruben's, the section skips non-solidified surfaces.

For Jonathan's, that super-thin cut separating the rib from the model creates a separation in the cross-hatching. From there you can switch to X-Area (in the modify x-hatching menu), toggle to the rib x-hatching then erase the x-hatching.

J
Jacek_Mydlikows1-Visitor
1-Visitor
December 4, 2015

there ia an old trick to worj this problem around

http://www.synthx.com/tom/sy_tip_9804.htm

http://www.mcadcentral.com/creo-drawing/15959-omitting-secti-n-lines-n-ribs.html

    K
    Kevin1-Visitor
    1-Visitor
    December 6, 2015

    ANother way is to create the section in the part and add it to the desired drawing view, in the drawing view erase them hatch, create a boundary for the desired hatch area on the view ( you'll also want to set the associate to view setting for the sketch geometry, and hatch the area. Gives more control over spacing and angle than just using a sketch in part mode.

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