Split a part?? From one ipt to two?

I need to take one part and split it into two. The primary reason for this is to be able to print a 12.5" part on a 3D printer with an 8x8x8 size limitation. It is a somewhat complex part, and I don't want to have to start over and make two things and glue them together later.

The other reason is that i have modeled a part as one solid body and it should have been two. A motor with an output shaft. This part is simpler, so I could easily make it agian, but I need to learn how to do this. Anyone?

Sketch split line.

Exit sketch.

Select Split and set to option Split Part.

Manage tab>Make Components to push out individual components and assembly.

After splitting you might add features to help bond together, like maybe pins (cylinders) and holes.

Keep in mind that 3D printing processes aren't particularly precise - so add a bit of extra clearance on the pins.

This tutorial shows step-by-step how to split a single solid into 3 different parts.

http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%202011%20Tutorial%2014.pdf

I just realized that one of the splits in that file might be far more complex than you need.

The other one simply uses one of the origin planes to split the part.

That tutorial doesn't show how to use a simple sketch to split a part.

If you have an open or closed profile sketch that completely tranverses the part - you can use it to split straight through.

Its not working

See attached pictures and the ipt for the motor. Sketch 21 is where is select for the split. Whats the deal:?

motor.ipt

Split should work, but something is wrong with the model that it doesn't, so

I'll show you how you it should have been done from the beginning and we will fix this part of the model -

Edit Extrusion5 and set it to Asymmetric (to send the rotor shaft back into the stator housing) and set to New Solid as shown.

(accept any error messages)

Now that you have two solids, Extrusion6 (and several other features) do not know which of the two solids they belong to.

Edit Extrusion6 (Edit Feature) and activate the Solid selection tool and click the shaft as the solid that the keyway (Extrusion6) belongs to). OK and Accept any errors.

Repeat for each feature that shows an error in the browser working your way down from top to bottom (some of them will start fixing themselves).

BTW - the Sweeps to cut those rings on the shaft should have been done with Revolve - Cut, just like on a lathe.

If you intend for this thing to move like a real motor you will have to go to Manage>Make Components to push out the assembly and then fix the assembly constraints.

I did it! Thankyou thankyou

Now that I have the new .iam, how can i make a constraint about the center axis and drive it, say 10,000 degrees so it looks like its spinning? This is what I've tried and had no luck with:

When you pushed out the assembly both parts were Grounded in position (see thumbtacks in browser).

Do not do not do not unground the motor.

You will need to unground the shaft.

You will then need to add a Mate constraint between the axis of the shaft and the axis of the motor. (simply select the cylinders)

You will then need to add a Mate -Flush constraint between the Origin planes of the motor and the shaft that are perpendicular to the axis (looks like XY planes in image, but not sure)

The shaft should now rotate in position when you drag it with mouse.

In the image you are trying to use a gear type motion constraint - this is not correct.

Add a Directed Angle constraint between a plane parallel the axis in the motor and shaft (looks like YZ plane).

Right click on this angle constraint after creating and select Drive Constraint, enter the number of degrees to rotate and click play.

You can also Animate Constraint this angle constraint in Inventor Studio.

Perfect. It moves. What does it mean when a part is grounded?

So now, I can model a gear, place it in the assy., constrain it to the shaft, add woodruff key and two c-clips, and be in good shape? I have been using the inventor studio a bit, and I know that I can animate constraints within it. At that time would I use the gear type motion constraint?

I need to know what constraints to place on the objects. See attached for cclip placement.

The Grounded sets the position of the "base" part.

Use Insert constraints for the c-clips. Mate Flush origin planes between c-clip and shaft.

Gears can only be made in pairs, if you only need one then delete the second gear.

I was thinking of taking this approach:

Instead of using the spur gear maker, just sketch two gear objects.

Can they be constrained in such a way as to rotate and look like they are intermeshing?

Yes, but it is far far far easier to use the Gear Generator than to manually create gear.

I am going to make the gears soon. I must first finish splitting the gearbox into two parts, a body and a shaft that turns. I followed the same sequence of steps you prescribed for splitting the motor, however I ran into much difficulty when trying to tell the ring slots which solid they belonged to (edit feature, solid). Attached are gearbox.ipt (original file, from which next 2 files were produced), gearboxbody.ipt, gearboxshaft.ipt, and there is an iam but the site isnt letting me upload it right now. No matter. See gearbox.ipt. Try to follow me here.......

There should be two ring grooves and one keyway on the .350 dia shaft. After making two separate solids, one of the ring grooves disappeared. I tried to make the sweep again out of sketch 20 (profile) and sketch 22 (path) and every time I try to do it, the rest of the part disappears. Whats going on? I thought I could follow the same steps as for the motor. Any ideas?

gearbox.ipt

gearboxbody.ipt

gearboxshaft.ipt

Its cool i figured it out.... just made the part again... thanks for the assist JDM