In this blog I’m going to show you a super easy and fast method for splitting a part (plastic injection molded part in this case) up into two parts (upper half, lower half).
The command we are going to use to do the actual “splitting” is the SPLIT command which makes quick work of this task. But a lot of times getting the curve/surface/etc that you want to use to split/cut the part with is the hard part!
One method to generate the curve to split with is to use the PARTING LINE command on the Mold Tools toolbar.
In this case we select the TOP plane to define the direction of pull. The key to getting this to put the parting line in the right spot is to use the “Split Faces” option!
This is exactly where you would most likely want to split this part so that it was moldable and didn’t get trapped in the mold (no undercuts).
After you hit OK, it will generate a CURVE that you can then use to make the surface you are going to split with.
Another method to get this curve that would give you absolute control if you didn’t want it at the exact division between positive and negative draft would be the SPLIT LINE command with the SILHOUETTE option and adjusting the ANGLE setting.
(See my last blog on using this command in detail… https://www.3dvision.com/blog/entry/2017/05/17/solidworks-surfacing-trick-for-mold-design.html)
Next you would use the curve generated with one of the above methods to create a RULED SURFACE that extends INTO the part enough to cut thru the wall thickness. The RULED SURFACE option of PERPENDICULAR TO VECTOR works great, using the TOP plane once again to define the vector.
Ok. Now time for the splitting…
Find the INSERT—FEATURES—SPLIT command. HINT: The easiest way is to search for it in the upper right corner of the screen!
Use the RULED SURFACE as the TRIM TOOL, then hit the CUT BODIES button.
If you just want the result to be a multibody part with the two separate halves in it, then just turn on the check marks for the resulting two bodies and hit OK.
(Make sure to TURN OFF the “Consume Cut Bodies” option!)
This command will actually let you make two separate PART FILES as well though!
If you want to do that, double click in the “File/name” column next to the check marks, browse to a location and give each part a name. Then when you hit OK it will go and create those part files on the fly.
Piece of cake to split up parts like this when you know this easy and fast method!