Slice and create two parts ?

[euphnut65]

Slice and create two parts ?

Often, I wish I could use a feature that I used to use in TurboCAD where you can slice a part with a plane and two parts would be created. While I'm sure it's a lot easier in a non-parametric program like TurboCAD (parrts are not named, just on layers), I would think it could be done in Alibre.

The parts could maybe split into an assembly(?), or maybe better just two separate parts. Maybe since duplicate parts are of the form xxxxx<1> and xxxxx<2>, the split parts could be xxxxx<A> and xxxxx<B>.

Any one have any opinions on this?

Thanks,
Eric

 

[Mibe]

Use booleans. This way the split parts also stays parametric to the original part...

 

[euphnut65]

Booleans?

Mibe,

Thanks for the pointer, but would you provide a few more details? I attempted to use booleans for another purpose, but scrapped it in the end since it didn't seem to fit the bill (rubber pads on the end of a metal fixture).

The example I was thinking of is to make a part that would be symmetric on a gripper where there would be two halves of a fixture to hold a cylindrical shaped object. Probably the same idea as a two halved mold, except the I want to reference the outside dimension (both halves) off of another part as well as the inside.

Thanks,
Eric

 

[z28tt]

I just ran into the same issue. A split command would be very useful, and most other packages seem to have it. After some late night thinking, my work-around is to insert a plane - I want to use a face as a splitting plane - this part is fabricated steel, and I need the assembly to trim itself automatically. On this plane, I just draw a box large enough to surround the part, and then do an Extrude Cut to get rid of the material below the plane. Works great, but it clutters up the drawing with another plane, another box, and an extra extrude command.

Andris

 

[jwilde]

I use the same work around as Andris, but it would be very nice if we could have a split command like the one I used to have in Turbo Cad. :!:

 

[moyesboy]

two ways to do something like this:

Create your one piece part.
Create a new part, and do a boolean unite from the original. This gives you a lump which is the shape of the orignnal one pice part.
Now cut that how you want.
You can do many extrude cuts and have a complex split line if you want, or just a planar one.
Now so that you don't need to define your cut twice, have it so the cut is defined only in the first part by creating the other half with a boolean unite of the the original, and then doing a boolean subtract of the first boolean part.
Do all the shape changes in the first one piece part. Do any edits of the split line in the first dependant part. The second part section looks after itself.

The other way is if you have configurations you can do the cut in the original part and then suppress the cut, but have it active an a configuration. Now with some clever dimensional changes to that cut sketch create another config where the other half of the part is cut away.

If you are creating a moulding that fits together two parts then you are best off using the boolean way and then you can model lips, pips and things on one half that are automatically mating with the other half.