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New Creo User

fdefilippi
1-Newbie

New Creo User

Greetings:

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

Frank

1 ACCEPTED SOLUTION

Accepted Solutions

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.

View solution in original post

18 REPLIES 18

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.

Best,

Toby

I like the CAD Quest Books.

Hi Frank,

You can get some help via the tutorials found at the PTC University Learning Exchange.  You can also, search for help in the Creo 2.0 Help Center or Creo 3.0 Help Center.  The other alternative is to contact PTC Universtiy (1-800-477-6435 > 9 Customer Care > 1 PTC University).

Thanks,

Amit

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

Hi Frank,

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, ...)

Hi Hugo-

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..

thanks

Frank

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.

Regarding Sketches:

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

Regarding Measure:

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?

...and to answer your question, yes, it will give the X, Y, and Z, and Delta (ditto) in relation to. a selected coordinate system.  You have to select the Csys and you have to manually activate the selection request by highlighting the field in the UI.

Creo rarely assumes things that are better selectable.  However, a default checkbox here would have been nice.

isn't the information give by the measure tool in Creo 2.0,3.0 confusing.i\I mean which is the x-coordinate,y-coordinate,z-coordinate.which is the projected distance ..with just one line showing a distance?

In Creo Elements/Pro 5.0 there where separate dimension lines for each coordinate.

In your screen shot you've specified that the measurement should be he distance as projected on the View Plane (in the center of the dialog).  This, by definition, is a 2D measurement so there can be no X, Y & Z.  You set this as a View Plane measurement by clicking the button that looks like a computer screen.

Typically, if you select the measure summary, then one item and the other, it'll give you several pieces of info about the pair, but not the Z, Y & Z distances like SW.  If you click the "Projection" field and then select a coordinate system, it'll give you that X, Y & Z.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Hi Frank,

Here is a quick reference guide that may help you get associated & familiar with Creo Parametric:

Quick Reference Guide

Thanks,

Amit

mbonka
15-Moonstone
(To:fdefilippi)

Welcome to community,

 

in order to make my input short as possible, will describe only keynotes. EVERYTHING needs much more investigation from your side.

 

Forum rules:

- fill tags in order to help others in searching

- mark correct and helpfull answer

- make separate topics for individual task. For example: Don´t ask about "constrains" in the topic called "New creo user" ... pls dont be angry to me

 

Generrall rules:

- keep your eyes open and be openminded

- don´t be scare to do mistake and take lessons from them ofc

- dummy is who don´t ask ... don´t be shy to ask something. Say THX if someone helped you.

- make your own knowledge library. Better to search your HDD then remmeber something .

- if you can´t find some icon ---> use search tool at the upper right corner

- use right mouse button to click secial items (top of arrow, lines in drawing) ---> many pop-up menus are hidden under RMB

 

Modeling rules:

- 3D model is INFORMATION HOLDER ---> drawing is "under" 3D model

- EVERYTHING IS ABOUT REFERENCES (from long time point of view)

- keep your references logicaly (use your brain before you click "something")

- NO EXTERNAL references are allowed

- SAINT RULE for companies and teams: "It is not import important if we ALL are modeling bad or good. Imprtant is, that WE ARE DOING SAME WAY. Only this way you can quickly take an orientation and understand your colleagues 3D models."

 

Knowledge sources:

- find your local PTC provider and pay for hotline support. My own is  Homepage - Aveng.eu ---  their hotline service is the best knowledge source.

- look into older models in your company and take some inspiration

- search this forum: CAD - PTC Community

- search Youtube:

    - basic assemblies:  E5 CREO Parametric 2.0 Assembly Basics 1 - YouTube

    - basic sheetmetal: Mounting Bracket || Creo Parametric Sheet Metal Tutorial - YouTube

- check as many totorials as you can:

    - E-Cognition Inc - Consumer Product Design/Development - Free Pro/E Wildfire Video Tutorials

    - Vladimir is the best one: Home | 4K Side - Pro/ENGINEER & PTC Creo Parametric Tutorials, Training, Mentoring, Customization an...

    - check Grabcad tutorials: Ptc creo parametric questions - GrabCAD

- search on Google

 

Some areas where you should focus on first:

- how does "Erease all displayed works "

- what is connection between part and drawing

- references

- parameters

- creo basic customization (config.pro; drw.dtl). See following list: Creo 3.0 M010 --- Configuration options In Creo you have large customization possibilities

 

Find your mentor:

- specially here are many persons, who "always have true" or at least very logical opinion. THX all of you...

     - Antonius DirriwachterTomD.inPDX

     - Tom Uminn

     - Vladimir Palffy

     - MartinHanak

     - David Schenken

     - sry if l forgot someone

 

Hope it can helps

Regards

Milan

TomD.inPDX
17-Peridot
(To:mbonka)

We have rules!

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.

View solution in original post

Coming from SW (I can't comment no the others), you'll find that Creo is less forgiving.  In the end, you may find that this is a strength rather than a limitation, but at first it'll drive you batty.  With nearly 20 years no Croe & Proe, when I have to use SW it takes me some time to flip my mindset and SW drives me nuts until I can.

SW anticipates your next move, makes a lot of assumptions about what you are trying to do and will generally take the input you give it and make something.  It takes the role of a helpful partner, anticipating and staying ahead of you.  Once you get used to it, you rely on it and its assistance.

Creo takes a wait for instructions approach. It is ready to do exactly what you tell it, but only what you tell it.  It doesn't assume much and generally doesn't try to do more than it's told.  If you don't know what to tell it, or you expect it to know what you're thinking (like SW tends to do), you will be frustrated.  Once you learn it's language and you learn how to describe explicitly what you want to happen, it becomes a very loyal partner, clinging to the instructions you've given and carrying them out explicitly.

There's nothing inherently wrong with either approach, but they have their strengths and weaknesses.  I find that features fail more often in SW, regardless of the care I put into building them, but they are usually easy and quick to fix so it doesn't matter much.  Feature failures in Creo can take more time to repair, because I have to be more explicit about fixing them, but if I build carefully they happen far less often.  Creo also gives me much more info on what failed and more options to fix them so that I have fewer failures down the tree.

If you keep this difference in philosophy in mind I think it'll help you. Personally, I find the level of control that Creo gives over SW empowering.  I may have to start slower, and build more deliberately, but I'm convinced that I finish faster and with a better design in the end.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Thanks again for your replies everyone and welcome once again Frank - ask and you shall receive.

Best,

Toby

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