Inventor General Discussion

Inventor General Discussion

Reply
Valued Contributor
pgcust
Posts: 70
Registered: ‎12-03-2007
Message 1 of 9 (1,158 Views)
Accepted Solution

Split 1 Body into 2 Bodies

1158 Views, 8 Replies
05-03-2012 03:20 AM

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

*Expert Elite*
JDMather
Posts: 26,528
Registered: ‎04-20-2006
Message 2 of 9 (1,155 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 03:39 AM 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

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Valued Contributor
pgcust
Posts: 70
Registered: ‎12-03-2007
Message 3 of 9 (1,146 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 04:42 AM 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

*Expert Elite*
JDMather
Posts: 26,528
Registered: ‎04-20-2006
Message 4 of 9 (1,138 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 05:09 AM 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.

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
*Expert Elite*
JDMather
Posts: 26,528
Registered: ‎04-20-2006
Message 5 of 9 (1,134 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 05:13 AM 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

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Valued Contributor
pgcust
Posts: 70
Registered: ‎12-03-2007
Message 6 of 9 (1,126 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 05:26 AM 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

Contributor
NCostelloe
Posts: 23
Registered: ‎12-08-2006
Message 7 of 9 (1,118 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 05:42 AM 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 Ultimate 2012 64-bit
Windows 7
Intel Xeon W3670 3.2 GHz
Nvidia Quadro 4000 1750Mb
8 GB RAM
Valued Contributor
pgcust
Posts: 70
Registered: ‎12-03-2007
Message 8 of 9 (1,103 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 06:06 AM in reply to: NCostelloe

Jd,

Here is the file.

 

 

Chris

*Expert Elite*
Curtis_Waguespack
Posts: 2,878
Registered: ‎03-08-2006
Message 9 of 9 (1,086 Views)

Re: Split 1 Body into 2 Bodies

05-03-2012 07:34 AM 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.

 

 



  solution.png  Did you find this reply helpful ? If so please use the Accept as Solution or  Kudos button below.





Announcements
Are you familiar with the Autodesk Expert Elites? The Expert Elite program is made up of customers that help other customers by sharing knowledge and exemplifying an engaging style of collaboration. To learn more, please visit our Expert Elite website.
Need installation help?

Start with some of our most frequented solutions or visit the Installation and Licensing Forum to get help installing your software.