I recently started a new engineering position (6 weeks), and this is my first time using Creo. I come from the Inventor/Solidworks/ Solidedge world I have been using Creo for 5-6 weeks and I am absolutely struggling mastering the basics to the level of frustration that I have leave my office and go for walks to calm down, and considering re-activating my job search. In the previous CAD packages they were easy to use and never required training. I've asked for some training (first time ever) but its gotten shot down, and in the meantime there is a concern that I'm not producing designs. To top that off I'm at a small company with myself being the only ME/Creo user, so I have no one to ask questions on the s/w. I started some one of the tutorials, but I stopped it after I was not getting the same results after multiple time. Can some PLEASE recommend a Creo for dummies book, any help would be appreciated
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Frank, I feel for you. Personally, I have a hard time recommending a new ME on Creo parametric specially if they don't have a mentor or proper training.
As a new customer, many VARs also offer a PTC University primer that does better than the free tutorials. It is actually well organized. I came back to PTC after a long time on Unigraphics NX. I updated my maintenance and received Creo 1.0 and 1 year of PTC University basic level.
What I don't see if comprehensive detail drawing training. This is becoming a lost art. But I fully understand you anxiety on this one. I stayed back on Creo 2.0 for this very reason. They experimented with a new UI on annotation and not only a few of us have openly stated that it missed the mark. For seasoned users, it is still fully functional if you get past the new UI.
USE YOUR SUPPORT CASES! When something is not working, submit a support case! You paid for this in Maintenance. USE IT!
And as you come up with what is keeping you from getting your job done, post here concisely what the problem is. If so desired, submit a support case at the same time. Often the forum will give you guidance before the support case has replied but it will give you two perspectives. Tech support has a way of finding some really obscure solutions to known Creo issues.
As for your management... yep, updating your resume may be useful, not because of Creo, but because of their attitude. Seriously, every upgrade from a known package required a 1 day session to understand the differences. A new package will require a training period. And Creo's learning curve is already pretty steep.
Find out if you have access to the free PTC University from your VAR. Tell your management that you require a reasonable training session. PTC will give you quote.
Otherwise, just stick with it. Creo really is a lot more powerful than the tools you've used. I just added SolidWorks to my resume and I can tell you that Creo is leaps and bounds more capable as soon as you veer from basic geometry.
Last but not least, feel free to post files here if you would like a simple review. Just activate the advanced editor here in the reply UI.
Welcome Frank; you have hit the jackpot regarding Creo knowledge.
Don't be afraid to ask questions: both about Creo as well as how to navigate PTC Community.
There are a lot of tutorials on YouTube and I have also used Leo Greene's E-Cognition website as well.
We have also used cadquest books from Steven Smith. CADquest Inc. - Pro/ENGINEER, Creo, and Windchill Textbooks
Can you tell us what kind of designs you want to implement or which part of Creo gives you trouble? (machined parts, welded parts, surface models, cast parts, ... assembly, drawing, configuration, ...)
I'm going to apologies up front because a lot of my engineering/ CAd experience is with Inventor/ Solid Works and Solid Edge. SO a lot of the command structures are the same, which I found easy to master 1-2 weeks.
I'm using the s/w for machined part, some optical mounts, I'll have to create drawings, 3d assemblies. Nothing overly fancy run of the mill small parts, simple things.
Some of the issues are:
Sketches, I can figure out how to create geometry, on a plane, but dimensioning it is something very different. Even after the first tutorial in Creo 3.0, I'm confused on how you dimension geometry, if I click on a line it no dim appears, not sure why, or dims I see I can select, delete or do noting. I just want to create a simple rectangle sketch place two dims and extrude. but I get these error message on not enough reference.
Measure. In a 3d object if I want to measure between two features on different Z axis height It doesn't display the x-y coordinate. I have yet to figure out how this tool works.
Constraints: No idea on how to use that tool, after 4 hours I just gave up.
I could go one and on..
Select the dimension tool, select the item to be dimensioned, then click (or middle click) to locate the dimension.
If you want to dimension between two points/vertices/curves select the first, then the second, then click to locate the dimension. Depending on what was picked and where was clicked it will create a dimension that is horizontal, vertical, or slanted.
You need to dimension to enough existing geometry to locate the part. Those are the references. Creo doesn't let the sketch float. Look for the sketch setup to pick enough references or add dimensions to existing geometry and it will add references for you.
I might be wrong, but I think the standard way in Pro/E to do something was to choose what to do first and then select what to do it with. In Creo you can sometimes select an object first, but in general I would say you first select a command and then you apply this command this should be most true for the sketcher.
In Creo you not only need to define the sketch plane but also how the sketch plane is oriented, i. e. which direction will be the top direction (Sketch Setup command) - this gives you two references minimum, but mostly four references. Sketch References can be separate from the Sketch Setup References, but with simple sketches the Sketch Setup References form the first entries in the Sketch References list (References command). Missing references may occur if you delete them, or you chose Sketch Setup References, that cannot be used for Sketch References.
Pro/E didn't let you exit the sketcher easily if the sketch was underconstrained. Since 15 years ago this should not happen any more since Creo places weak dimensions and constraints automatically to get a fully constrained sketch, but those dimensions are weak, meaning they can disappear automatically if you place your dimensions. You can make weak dimensions strong (context menu). Creo checks that strong dimensions and constraints do not contradict each other and asks you what to do if they do, but does not let you place contradictory constraints (which a strong dimension is part of). You can still drag around sketch entities constrained by strong dimensions. You can lock a dimension to prevent accidental movement of sketch entities.
relevant config.pro option: sketcher_auto_create_references
relevant Creo Parametric Option (Sketcher area): Automatic reference creation from selected background geometry
In the Measure: Summary tool there is a black triangle on the right side that gives you more options. In the expanded tool you can expand again at the bottom, there are all measurements listed.
You can also click the "+" symbols in the graphics window, this also lists measurement details (x, y, z coordinates for vertices, for example).
You might also be interested in the Projection option this projects a measurement onto some reference.
As far as my experience goes Creo is very strong on placing reference features. I try to focus on those to constrain my designs. In essence I would say you create your references beforehand and then you place your sketch. And I think you should keep your sketches simple, or the Sketcher's auto-constraints feature/requirement can make editing your sketches a pain.
I am not sure what you mean by "Constraint Tool".
I'll review what you wrote Hugo thanks.
In most CAD systems I've used "Constraints" refer to mating one part to another in an assembly.
In regards to Measuring in the screen shot below if I take a measurement between two holes it does not list the x-y distances between them. Again in past CAD program it would list that info so know the distance. very helpful in my opinion. Does Creo have that function and I'm not using it correctly?