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Split 1 Body into 2 Bodies

8 REPLIES 8
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Message 1 of 9
pgcust
4297 Views, 8 Replies

Split 1 Body into 2 Bodies

In the attached file you will see that the last op in the browser is cut Thru_1.

I am trying to split this into 2 bodies(keep cut the piece i have removed),Is this possible?

 

Thanks

chris

Inv 2010

8 REPLIES 8
Message 2 of 9
JDMather
in reply to: pgcust

I don't see a Split feature in that part.

Your sketch for a Split is on the wrong plane.

You simply need a U shape sketch on the YZ plane and select Split Part option to have two solid bodies.

 

 

Split Solid.png


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Message 3 of 9
pgcust
in reply to: JDMather

JD,

The Cut is staggered, so i cannot go straight through.I could not do a split in the file as i could not get the shape that i needed.

 

 

Chris

Message 4 of 9
JDMather
in reply to: pgcust

Let me take another look.

Of course the split can be made - it is simply a logical problem of setting it up correctly.

This one is trivial.


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Message 5 of 9
JDMather
in reply to: JDMather

OK, I took another (longer) look.

Edit your Cut Thru_1 extrusion.

Click New Solid and Intersection.

OK.

 

New Solid.png


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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


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Message 6 of 9
pgcust
in reply to: JDMather

Jd,

Thanks ,I have lost the sweep in the new body,should i just rearrange the order of the design.(Split part then sweep )

chris

Message 7 of 9
NCostelloe
in reply to: JDMather

JDMather's pretty much nailed it, but it won't quite get you there. (cool trick by the way to make a new body!) The step he just explained, you need to do at the start to make 2 bodies. You'll need to re-use that sketch to extrude away that new body in body1. Then make all your holes. When making your sweep, you can select more than one body to go through to make it easier.

As he said, it's just a matter of setting it up properly...

Nathan Costelloe

Inventor Professional 2022
Windows 10
Intel Xeon W-2133 3.6 GHz
Nvidia Quadro P4000 16Gb
Message 8 of 9
pgcust
in reply to: NCostelloe

Jd,

Here is the file.

 

 

Chris

Message 9 of 9
Curtis_Waguespack
in reply to: pgcust

Hi pgcust,

 

Here are some quick steps and a sample file to get what you're after.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

 

  • Use the Copy Object tool and copy the current solid body as a Composite surface
  • Expand the Solid Bodies folder in the browser and turn off the Visibility of the existing solid body
  • Use the Sculpt tool to turn the composite surface into an New Solid body
  • Extrude the sketch and use the Intersect option to keep only the material that intersects the sketch and the solid body
  • Expand the Solid Bodies folder in the browser and turn on the Visibility of the both solid bodies
  • Use the Combine tool and choose the first solid as the Base and the  second as the Toolbody, and be sure to select the Cut button and the Keep ToolBody option
  • Expand the Solid Bodies folder in the browser and turn on the Visibility of the both solid bodies again.

 

 

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