Unable to extrude projected sketch
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Unable to extrude projected sketch
Hello, I have a projected sketch that is on a flat surface parallel to the original sketch. However, when I use the extrude command I am unable to use my projected sketch as a sketch to extrude. Is there some trick to using projected sketches? It appears as if it's just a normal sketch but won't let me do anything with it.
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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.
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
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It would be helpful for trouble shooting if you could take a screen shot of your sketch.
What version software are you using? Any other pertinent details that might help us help you.
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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.
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You can do all of this in one multibody part and use a Boolean subtract to get the text cut out in the base part. You can then export the two bodies as parts and assemble them if needed.
Take a look at some examples in this thread where they are building multi body colored logos.
Re: Creo Parametric Community Challenge 6 – Sketch... - PTC Community
Involute Development, LLC
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Specialists in Creo Parametric
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Thanks for the input, I will look into this method.
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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"
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I'm lost on this method. I'm unfamiliar with the merge/inheritance feature so I did some googling but didn't come up with a solution that worked for what I was trying to do (or duplicate what you did in your tree).
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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.
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Thank you for the explanation,
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I just did a simple test (creo 6). I sketched a random shape and then projected it to another parallel surface. I am not able to use that projected sketch directly to create a cut or extrude from.
Depending on your specifics, you can create a sketch on the desired plane and use project from within the sketch command.
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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.
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What's the point of a projected sketch if it's not even a sketch?
I do know about the loop command under project. However, that allows you to loop 1 character at a time. If I have 100 characters to project that is going to take quite some time and be quite annoying. Especially when I already have a controlling sketch with all those characters in it.
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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.
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
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This is very helpful, thank you.