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Ketan_Lalcheta1-Visitor
1-Visitor
May 6, 2016
Question

How to use section of part into assembly drawing

  • May 6, 2016
  • 4 replies
  • 3565 views

Hello,

Is it possible to use section of a part file into a drawing file of assembly?

I am getting only cross sections defined into assembly file for a view present into drawing. How to get section of part file into below list:

Section.png

Thanks and Regards

Ketan


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4 replies

Dale_Rosema
23-Emerald III
Dale_Rosema23-Emerald III
23-Emerald III
May 6, 2016

If you bring that part into the drawing, you can show it as a cross section by itself, but if you only have the assembly file, it will show a cross section of the assembly. You may be able to "hide" some of the parts in the drawing.

    S
    23-Emerald III
    StephenW23-Emerald III
    23-Emerald III
    May 6, 2016

    You can't use part sections in your assembly BUT you can make a section in your assembly and EXCLUDE all the other parts of the assembly so only the part you are interested in seeing section is sectioned.

    1. create the section in the assembly

    2. create a drawing view in the orientation so show the section and add the section to that view. complete the view dialog

    3. In the annotate tab, double click on the x-hatch to get the x-hatch properities menu manager to pop up.

    4. Use the EXCLUDE option and NEXT on each part cut by the x-section except don't exclude the part you want to see cut.

    5. hit done on the menu manager and regen the view. it never updates fully until you regen the view.

    D
    dschenken1-Visitor
    1-Visitor
    May 7, 2016

    The other suggestions are as good as possible.

    One reason that sections apply only for the part or assembly it is defined in is that otherwise there could be multiple sections with the same name in higher level assemblies. Another reason is that if multiple identical parts were assembled, then there would be competing sections of the same name from the same source. The last reason I can think of is that the section has to be evaluated for the items it intersects and the part doesn't have a link into the assembly structure to create that intersection, especially if there were multiple identical parts in an assembly where a part section might intersect another assembly duplicate of itself.

      M
      manjunathrv17-Peridot
      17-Peridot
      May 9, 2016

      Ketan,

      The simplest solution is what is mentioned by Dale to add part to the drawing and show its section there.

      IF this is not feasible for you, then try to create a simplified rep showing only the part that you are interested in and exclude all the other parts.

      Then this Rep can be used in the drawing with the section showing only the part you are interested.

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