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HamsterNL
HamsterNL18-Opal
18-Opal
January 23, 2020
Question

Solidify and sheetmetal

  • January 23, 2020
  • 4 replies
  • 3140 views

When working with a sheetmetal part, solidify only gives the option to remove material, not to add material.

 

Is there perhaps a secret config option to allow the addition of material in a sheetmetal part?

 

The workaround for now is to start with a solid part, then use the solidify feature, then convert the solid part to a sheetmetal part.

4 replies

HamsterNL
HamsterNL18-OpalAuthor
18-Opal
January 24, 2020

Another way to get geometry into my existing sheetmetal part is by using Inheritance.

 

Inheritance does work in sheetmetal, but overlapping geometry can't be merged by the Merge Wall feature. So I first need to remove material if I have any overlapping geometry, then use a second inheritance feature to add material.

S
slolli10-Marble
10-Marble
February 4, 2020

Another option is the following

  1. Create a new part (sheetmetal)
  2. use Copy Geom to bring in a surface/quilt 
  3. Create Offset Wall type (Model > Editing > Offset)
    • Offset =0
    • Select direction to set thickness
    • Set wall thickness
    HamsterNL
    HamsterNL18-OpalAuthor
    18-Opal
    February 8, 2020

    Hi @slolli,

     

    Thanks for your suggestion!

     

    I have tried your method, but I am using the "All Solid Surfaces" with my Publish Geometry, and I can't create the Offset Wall Type in my part. There are some extremely great advantages for me to use the All Solid Surfaces option, I can't publish just one surface (to give you some more information, I am (un)supressing completely different geometry within my Publish Geometry part).

     

    HamsterNL_0-1581155244357.png

     

    S
    slolli10-Marble
    10-Marble
    February 10, 2020

    Hi, the steps I gave as an option are under the assumption you are bringing in a surface quilt that has no thickness.  For example, if you had a complex contour and you bring in only one side of surfaces. See below

     

    Solid part looks like this, green highlighted surfaces is what I select with the Copy Geom.

    slolli_0-1581346921626.png

     

    I only selected certain surfaces (on one side) of the part so it is a zero volume quilt I am starting off with in the sheetmetal part

    slolli_1-1581347122856.png

     

    Alternately, if you do bring in all solid surfaces, you should be able to use the Special Handling area to remove surfaces that are considered for the Offset operation.

    slolli_0-1581347496599.png

     

     

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