How to design a mould in Catia V5 and Solidworks 2011 from an existing part file?
Here is the Tutorial!
Attachments078.SLDPRT, 663 KB
First of all open any part file in Solidworks.
Choose Mold tools tab and then parting line option.
Under direction of pull select the pulled surface.
Choose Draft analysis for positive and negative draft analysis.
Choose Parting line option.
under parting line option choose an edge like i selected for parting line
Choose propagate for SolidWorks to automatically select the parting line to form a closed loop
Click OK and you can notice a blue edge. Now choose Shut off surface option to close the open holes etc.
Solidworks will automatically select the edges to form shutoff surface in direction of pull. Click OK then. You can notice surface to be formed on holes.
Now choose parting surface. It will be the surface which will be the surface to split core cavity body.
Solidworks will automatically select the parting line. if don't you can select the parting line. And change the parting surface distance to something greater like 14.6mm etc. And choose OK. You can notice a surface around the parting line.
Now choose tooling split to form the core cavity bodies mould.
Select the parting surface formed as the sketch plane.
Sketch workspace will be opened.
Now draw a circle between the edge of the parting surface and the parting line.
Choose OK. Now you can notice the formation of the tool cavity around the body.
Change the view to Isometric if needed.
Click OK. Now you can notice that the body was enveloped in another body.
Now hide the parting surface. If Needed.
Now go to Insert>>Features>>Move/Copy...
Translate the upper body in Y axis.
Repeat the same step for the lower body and u are most probably done.
Additional information:- Scaling the body is necessary before making mould to counter shrinkage.