Cutting on a plane?

[jennpeeler]

Ok... so there is a question about cutting already here, but mine is slightly different. In a part, if you have a work plane that is not parallel with any of the other planes how do you cut off (completly obliterate) the part of the object on one side of the plane. I cannot find a command to do this so I hope someone knows :)

[FourPenguins]

I haven't hit inventor since last year, but it seems like the easiest way to do it would be to make a sketch from your workplane and just extrude/cut a large square/rectangle.

[Al Skierkiewicz]

Why not create another plane? Then you can wipe what you don't want and then follow up with deleting the plane.

[jennpeeler]

My biggest problem is that I cannot get Inventor to extrude along my work plane instead of along the x/y/z planes... my plane is diagonal to the standard three.
I'm not sure if this is possible... but if it's not is there some other way to make a cut across planes in Inventor?

[Greg Needel]

If you are trying to extrude along a plane the best bet is to create another work plane 90deg's from the origional, make a sketch on that plane in the shape of what needs to be cut away and extrude it.


If you could post some screen shots of what you are doing we might be able to help you better.

[negfrequency]

If you are trying to cut on a plane, you will probably find it easier to use the "split" or possibly "replace face" command that are offered for that same reason in the part features menu. The replace face is EXTREMELY useful for operations like this since you can make extrude lines to form bent work planes from the side view and then remove all material up to that surface.

Split can be useful if you want to salvage both parts of the piece. For example in my CIMS class we had to make the top and bottom of a container using one block. Since we'd separate the block in real life our teacher wanted us to split and save both parts on the CAD program(we used inventor of course)

[CraigHickman]

Just making a large shape, and picking that profile to extrude should work, if I'm understanding the problem. If not, a screenshot would allow us to help you out better.

[Andy A.]

Split is probably the easiest way to do what you want. I think it's pretty straightforward, but I'll include a couple of screenshots for clarity. It sounded like you didn't have any trouble getting the workplane put in correctly, so I won't cover that.

http://i122.photobucket.com/albums/o249/Local_ifr/Split_command_result_example-1.jpg

Make sure to select the correct method. The one I have selected will delete everything in the direction of the arrow. The other method is a little more complex and would allow you to keep the other side and split the part into two. It doesn't sound like this is what you wanted.

http://i122.photobucket.com/albums/o249/Local_ifr/Split_command_result_example.jpg
The part after the operation. The split is considered a feature, so editing and suppressing it is easy.

I use this a lot in a class that requires designing cast parts. As a cast part has two states- when it comes out of the mold and after machining, you have to supply drawings a models for both states. This is just one way to quickly switch between two states of a part with out getting into complex spreadsheets to drive parameters. It's also considered a little more acceptable then cutting with extrusions, something which was almost never acceptable on a class project.

There is almost always a dozen ways to get something done in Inventor. This is just the one that I would use knowing nothing else about it. Replace face is another good method.

Also, you should be able to place a sketch on the workplane, and cut/extrude from that sketch. The direction of travel should be 90 degrees from that sketch, and not from the origin planes. I don't know why that wouldn't be working for you.

-Andy A.

And yes, the date and time on my computer are correct. What better to do at this time of the morning then play around with Inventor?

[jennpeeler]

Ok thanks Andy A, that worked... I didn't realize such a command existed... thanks everyone who had suggestions... :)