Copying A Shape From A Part To Another

[mgajewski]

Hi

 

I wonder if there is a way to copy or move shapes from part to part (just like copying/moving parts between assemblies)?

 

I don't think it can be done directly (it would be awesome if it could) but does anyone know of a workaround that accomplishes essentially the same thing? Even if the resulting part becomes "dumb" after the operation...

 

I am working with a complex imported part that I have applied some shapes to and now I have another imported part which I'd like to modify the same way but do not want to go through the process again and anyway I am not sure I could duplicate it exactly...

 

Mark

[Cary OConnor]

There is an Add-on tool that does this. It will basically copy the selected shapes and paste them under the selected part to move them too. You will need to position them after the copy since it will paste them in the same location from where they are copied. Close IronCAD and then go to ..\Program Files\IronCAD\IRONCAD8\ICAPI\Samples\bin and register the ICAPICreate.dll with Regsvr32.exe under C:\WINDOWS\system32 (register means open with). Start IronCAD and Go to Tools\Add-in Applications and select the IC Create and select ok. On the toolbar that pops up, you have the copy command. Read the ICAPI Help under Docs for more samples.

Cary

[B. Ludin]

You can also drag the shapes to a (temporary) catalog and from there to the new part. That's a useful workaround in many (but not all) situations.

 

Beat

[janderson]

In the same vein, you can Combine the shapes you want to re-use. Make sure the anchor point of the combined shapes is at a place where you can snap it onto the next part you want to put on. Then, select the combined shapes and put them in a catalog. Note: A peculiarity of Ironcad 8.0 is that you can't use the Triball snaps to move the anchor point of the combined shapes in the scene, but triball snaps to move the anchor point will work in Edit Catalog Item. When the anchor point is in a good place to snap onto the next part, simply drag the combined shapes out of the catalog and onto the part.

 

 

I use this type of thing for plastic injection molds, where I take the part, and a positive of the the sprue and runner system, then Boolean parts and Combine shapes as necessary to create one single part. Then, drag the whole thing into a catalog when selected as a shape. Then, use 'Edit Catalog Item', and apply the shrink factor as a multiplier on the shape's handles, then, use Shape + Set Operation to change the resulting enlarged shape's action to Remove Material. Now I can drag it onto the mold and create my cavities.