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How to create a sheet body based on a solid body?

Experimenter
Experimenter

I have a simple 3D airfoil that is a solid body structural model. How can I generate a sheet body based on it?

 

I'm really new to NX. Have searched extensively online about this but couldn't find anything. Any help would be appreciated. Thank you!

1 REPLY

Re: How to create a sheet body based on a solid body?

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

Hi @jl477,

 

Here are several suggestions.  Research each one to see which suits your application.

 

1) Menu > Insert > Offset/Scale > Offset Surface

Enter zero (0) for the offset, set the Output to "One Feature for All Faces" and set the Face Rule to "Body Faces".  Select the body and choose OK.  A single sheet body is produced.

 

Edit:  I tried Offset Surface again and it produced a solid body the second time.  I probably orignially used it on one of the sheet bodies below when trying to find alternative (simpler) solutions Smiley Happy

 

2) Menu > Insert > Associative Copy > Extract Geometry.

Set the Type to "Face" and Face Rule to "Body Faces", check "Hide Original" and select the solid body.  This will create a separate Extracted Face feature for each face.  Then select "Menu > Preferences > Modeling" and on the General tab change the Body Type to "Sheet".  Finally select "Menu > Insert > Combine > Sew" and sew the Extracted Face features together to make a single sheet body.

 

3) Menu > Insert > Associative Copy > Extract Geometry.

Set the Type to "Body", check "Hide Original" and select the solid body.  Then select "Menu > Insert > Combine > Unsew" and select one of the faces.  You might have to change the Face Rule to Single Face.  Then select "Menu > Preferences > Modeling" and on the General tab change the Body Type to "Sheet".  Finally select "Menu > Insert > Combine > Sew" and select the main body and then the unsewn face back together to make a single sheet body.

 

Regards, Ben