Modeling patterns in Solid Edge 2

[xj5373]

Hi,
As a complete new start to Solid Edge I am hoping to use it to model patterns for lost wax casting. What I want to do is to model the required part in 3D, then split the model into two halves along the selected parting line. I think I am ok with this first step. The next bit though is I want to change the model from a 3D shape to a 3D cavity in a solid. In other words I want to subtract the half solid model from a block representing the stock material. Is this possible or do I have to model the pattern from the start?
Grateful for any tips you can give.
Ian

 

[donyoung]

Hi,

one solution:

- open a new part
- insert the part in question but as Construction Body
- activate Surface Bodies
- Optional apply a Shrink Factor by which the model
should be enlarged to cater for any shrinkage

OK

Now model a simple Protrusion so that it encompasses the inserted
part. Put the profile on a suitable face of that model or use a
reference plane that suits

Then use Boolean Subtract and subtract the inserted model from
the just created Body.

that's it

dy

 

[xj5373]

Thanks Don, I will give this a try and see how I get on.

Ian

 

[Bhaveshn]

Don,
When inserting a part copy, how we can locate the part position relative to exisitng geometry. There is option of cordinate system, but it doesn't locate relatively.
can we define its position as we do in assembly?

 

[donyoung]

Hi,

within the receiving part you can define a coordinate system and
use it during insert part copy. The inserted part will then
be put with it's 0,0,0 point as well as with the axis coincident
to this coordinate system. The coordinate sytem may be defined
either realtive to the model space or be based on the geometry
of an already existing part. In the latter case ist will follow
the move of the part the coordinate system is attached to.

By changing the values of the coordinate sytem you may be able
to turn/move the inserted part

The other option is to modify the part by using the direct editing
(modify) commands 'Rotate' or 'Move' (select body instead of face
in the pulldown) but it's a bit cumbersome ...


HTH

dy

 

[xj5373]

Hi,
Just thought I would report success! 2 parts modelled and then inserted as construction objects into a new part representing the pattern blank. I set up alternative co-ordinate systems in the blank to allow me to position the models as I wanted. Using the boolean command enabled me to remove the inserted parts leaving the required cavity in the pattern....voila!
To get the other half of the pattern I retraced my steps and extruded the pattern blank in the opposite direction, did the insert, did the boolean and then I had the other half of the pattern. Last step was to turn the part over to get the z axis in the right direction. Not sure if I did this the best way but I opened a new file and set up a corodinate system with Z in the opposite direction and then inserted the part into that. I couldn't find a way of moving or inverting the part directly but I am sure there must be a way....
I am now heading for my CAM software and my machine.
Thanks for the excellent help.

Ian

 

[kjoiner]

Ian,

Another trick you could try that will save a step or two is to use the split part tool. This is commonly used for molded plastic parts where you can model the entire part in one piece, then create a plane to define the parting line and use the split part tool to create two parts that represent the two halves that that make up the tool. The master part that you boolean subtracted the pattern from will remain one piece and will drive the two halves. If you change the pattern or move the parting line, the two part files will update automatically. This will save you from having to keep up with parting line locations maually. Using the split part command, you can also break up the part into more than two pieces.

Kyle