Inventor help: split a solid

[DonRotolo]

I need some help with Inventor (Professional 2011 Student Edition).

I have a solid that looks like a barbell, and I want to split off some of one end of the 'barbell'. One image below shows the end in question, and the work planes (in yellow) at the places I want to split.

When I use the Split command, it wants to split off in the plane, but along the entire length of the part, not just the one end. The red plane shown in the second image shows what it wants to split off (not perfectly clear, but the split does extend through the far end "barbell").

How do I split off these bits at one end but not the other?

[scottydoh]

I've never actually used the split command, and I know this maybe isn't the "right" answer, but just a thought. Could you use a cut/void extrusion to remove the sections you're talking about?

[Duke461]

Originally Posted by scottydoh

I've never actually used the split command, and I know this maybe isn't the "right" answer, but just a thought. Could you use a cut/void extrusion to remove the sections you're talking about?

I also don't have a ton of experience with split, and i don't have a computer with Inventor nearby by me so for now i can't tell you how to do it through splitting. However, you should very easily be able to make two lines, one for each line the work plane cuts through, and do a to-next extrusion cut.

[scottydoh]

Originally Posted by Duke461

I also don't have a ton of experience with split, and i don't have a computer with Inventor nearby by me so for now i can't tell you how to do it through splitting. However, you should very easily be able to make two lines, one for each line the work plane cuts through, and do a to-next extrusion cut.

That's exactly what I was thinking. Just an update, I tried it out, and I have a feeling that you really can't control the split amount, seems from the description that its good for things where you want to split the entire mass in one smooth step. I'd just sketch a line on the surface and use the cut extrusion "to-next"

[Al Skierkiewicz]

Don,
Are you trying to use a plane to initiate the split? You might try using a 3D object like a box with a minimal height for the splitting boundary. In Autocad, I would use this method with the 3D editing 'subtract' command to remove the unwanted parts.

[slijin]

Do you want to use the parts you split off, or simply remove them from the piece? If the latter, then an alternative you could try is creating a surface sketch on the end of the piece, then extruding that sketch to remove said pieces.

[Brandon Holley]

In SolidWorks I would do this...

Create a couple of surfaces to create the boundary of the split. Stitch the surfaces together to create 1 trim "tool" and then use the split command. I'm not sure if its the same for Inventor, but its gotta be similar. SolidWorks also allows you to pick more than one surface/plane to create your split. I choose to knit because I think its a bit cleaner. Essentially you need to create a split "tool" so you can do the split appropriately.

-Brando

[MechEng83]

This is actually a common mistake when using planes in any 3D CAD package.
Even though the visual representation of the working plane appears to be limited to a specific rectangle, in actuallity, it goes to infinity in every direction. Thus, when you try to use the plane to "split" one end, it is splitting along the entire plane.

I suggest either creating an actual surface in the vicinity of your split or a 3D extrusion, depending on what your final intent is.

[inventor_phild]

Don,

Sounds like you have a solution for the work flow. Unless you need to use the top part of the barbell, then the Extrude option works well.

[Ankit S.]

EDIT: The following is for Inventor Professional 2012, I'm not sure if it is the exact same in 2011, but I don't think its too different.

Try this: Instead of using the "Split Solid" Feature, try using the "Split Face" feature, and specify only the faces you want to be split, basically just the ones on that one side. Unfortunately, this wont create a new solid, so if that is what you want, you will probably have to do something else.

Hope this helps!

[JD Mather]

Originally Posted by BeltSanderRocks

Try this: Instead of using the "Split Solid" Feature...

This doesn't answer the question or solve the problem.
The problem has already been better defined in that the visual of the plane is just that - the plane actually extends to infinity (or as far as the computer can calculate) in all directions. This is true in Inventor or SolidWorks.

The easiest solution (in SolidWorks or Inventor) is to create a U shaped sketch on the perpendicular plane and use that to split the part.

Alternatively extruded rectangles with Cut option can achieve the same results.

Attach the ipt file here if you can't figure it out.