1 ACCEPTED SOLUTION
Accepted Solutions
This is one method to create the geometry using multi-body functionality. It is very efficient, and no projection of the sketch required. See the enclosed assembly and parts. This is all driven from the master model "mb_master.prt". Creo 7 models enclosed. All changes to the text and the plate can be driven from the master model.
I am using Creo 7.0.9.0
I come from SolidWorks and this is how I handle this kind of situation so please let me know if I should go about a different method within Creo.
I am 3d printing a multi color object which requires a multi bodied part. What I do is create my 'base' part with cut extruded text, then create an assembly and then assemble my 'base' part. I will then create a 'text' part but don't create any features. I assemble the 'text' part in my assembly. Within my assembly I will activate my 'text' piece and project the text sketch from the 'base' part, then extrude in the text. This gives me two parts to export as an stl and then print with multi colors.
However, in Creo I can either use the loop project command within in my sketch command and select each character 1 at a time (super time consuming when you have lots of text) or I can create a projected sketch. But the projected sketch does not allow me to create an extrude.
I can't screenshot what I am actually working on but here is a simplified version of what I am trying to do:
I need to fill in the words 'test'. You can see I created a projected sketch under test-piece-2 (based off the sketch on test-piece-1). It just won't let me extrude it.
Just another quick test (Creo 6, no multibody). I created a block part, I created a "text" part.
In the block part, I used Get Data - Merge/Inheritance function, set it to remove material and then put the text part where I needed it.
At work, we are still on creo 6 so we haven't gotten in to multi-body parts, so my method is using boolean operations via Merge/Inheritance features shown in the model tree as "external cut out"
For the simplest example. I built a simple block.prt and a simple text.prt. 2 separate part files.
Open the block.prt
Get Data - Merge/Inheritance - then "remove material"
Then pick the Open folder, choose the "text.prt" and you basically assemble text part on to the block part (same as assembly placement, just within a part).
You can use the preview button from within the "component placement" dialog to see the placement.
Hopefully that is enough to get you rolling. There are other ways to do this, likely better ways, especially using multibody.
Hi,
if you project a sketch the result is a projected curve but no longer a sketch.
Sketch-based features only accept sketches as an input.
What you can do is to create a new sketch in the other part ans inside the sketch 'grab' the sketched lines of the original sketch via the sketcher function 'project' with the option 'loop' for ech letter.
This sketch can then be extruded and will follow any modification in the original sketch.
This is one method to create the geometry using multi-body functionality. It is very efficient, and no projection of the sketch required. See the enclosed assembly and parts. This is all driven from the master model "mb_master.prt". Creo 7 models enclosed. All changes to the text and the plate can be driven from the master model.
