Hi guys.

I work in a foundry and I am responsible for modeliing castings before simulations. I normally start the design as specified in the drawing supplied by a customer. I then make contraction allowances by using part copy. Enlarging the part with part copy gives me a problem. If a part has a hole, part copy generates a bigger hole that is not symmetrical to the hole of original design when what I  desire is a smaller hole that si perfectly symmetrical to the original hole. This misalignment is clearly visible. I was hoping solid edge has a function that would enlarge the whole volume accordingly. If this is possible , can anyone help me in getting it right. 

Insert the part copy without scaling. Then use Surfacing ->Offset and then choose “body” for selection type. At the end attach the offset to the design model – right click on the Offset in PathFinder window and click on Attach in shortcut menu.

Attachments
 Offset_body1.JPG [94 KB] ::
 Offset_body2.JPG [88 KB] ::
 Offset_body3.JPG [88 KB] ::
 Offset_body4.JPG [106 KB] ::

Thanks a lot savata. It is extactly what i was looking for.

I did not get the last part right. Where I am supposed to right click offset and click attach.

Wer are still using ST2 package and i wonder if i can achieve that with this package

Cheers

There is a way to make it in ST2.

1. Start new Traditional part.

 2. Click Part Copy button and in “Part Copy Parameters” window you must choose: Copy as Construction Body!!! (By default this option is set on Copy as Design Body). OK.

3. Go to Surfacing menu -- > Offset. In Select Step cell choose “Body”. Then type the offset value and click for the direction in which the offset to be done.

 4.The last step is to make a solid from the new offset surface. Right click on “Offset1” in PathFinder window and from the shortcut menu choose Make Base Feature – this makes a base future from the selected construction.

5.Cheers!   

Attachments
 Offset_Body_ST2.JPG [136 KB] ::

Another way - if the body you want to offset is Synchronous part:

1.       Open this Synchronous part and save it with another name. Part Copy doesn’t work in ST2 when you are in Synchronous mode.

2.       Again -  Surfacing menu -- > Offset , in Select Step cell: “Body” ……………………….. OK.

3.       Right click on “Offset1” in PathFinder window and from the shortcut menu choose “Attach”.

One more way to make offset body – in Traditional Part:

1.       Build or open some kind of model in Traditional Part and offset the body (Surfacing --> Offset, etc).

The result is construction offset geometry which is not a part of the solid body.

If we want to make this construction geometry solid, there must be no other solid geometry.

So, we do the following:

2.       Right click on (the last) “Offset” in PahFinder window and choose “Drop Parents”. Now the current solid geometry can be deleted.

3.       Delete the solid geometry. Now there is only the last offset geometry.

4.       Right click on “Offset” in PahFinder window and choose “Make Base Future”.

The bad thing is that the build history of the part is deleted, so maybe we must save two files with different names – one file with build history of the part and another with the offset solid.

The good thing is that when we start using the Synchronous Technology we will not care too much about the build history.