Learning PTC Creo.......... 3

[CAD2015]

Hi,

I am very familiar with Catia, SW and NX (2D and 3D, chassis and electrical).
I am interested in learning PTC Creo. Would my previous CAD system experience help me to achieve my goal in a week or two?

Thanks,

 

[dtimberlake]

Will you be making large assemblies and then detailed drawings with BOMs and families of parts?

Some folks (including engineers) I respect held ProE in very high regard regarding power and features, and considered SW unsuitable for for REAL engineering.

.My experience is dabbling with ProE/Creo at this company for a decade after Cadkey and Solidworks previously.
Mostly Layouts for investigation often from others' modelled assemblies and models for FEA.
I think Creo as new as 2.0 is prickly, arcane and inscrutable. I still like it.
Two 40 hour weeks armed with Tutorials and frequent referrals to online help might have got me making parts, modest assemblies, and maybe drawings.

The designers here that started with Creo and used it for years hated when we went to Inventor a couple of years back. Many still do.
(some alsoget apoplectic and threaten to retire when asked to revise an ACad 2 D drawing of a single component.)

My SW is 2007-ish and Inventor is 2021 with many very recent updates. I think today's Inventor's interface is much like SW , with some very useful additional features.
Inventor around 2001 was clunky as hell when we evaluated it and SW.

 

[3DDave]

"in a week or two"

No or probably not.

You can go to the PTC website and find the help documentation for all the features online for free and I suggest to people that they read as much of the documentation as possible, even if they feel they cannot memorize it. It helps to get the names of features and functions and gives an idea of what the software can do, decreasing the time to find how to do what they want to do.

See https://www.ptc.com/en/support/help/creo

Other than that it is difficult to tell. Often people get used to what they start with and keep trying what used to work and are frustrated when the other software is different.

One of the main complaints I have heard from those taking up Creo after other software is how inflexible it appears to be. Yes. It appears inflexible because it is not making a ton of assumptions that can cause weird problems later on. Some don't like the need to consider how items will be dimensioned and how features will relate to one another.

What I liked about using Pro/E, Wildfire, Creo was that it operates a lot like an interactive programming language. I tell it what I want and it does it. That also means sometimes debugging skills are required because I told it to do something and it did what I told it to do and not what I wanted.

To offset this there are diagnostic tools.

An example of a problem that users create for themselves: They want to put a fan in a wall. So they go to the assembly and roughly position the fan where they want it. Then they activate the wall part and use the fan as the alignment for cutting the mounting holes and air hole in the wall part. These are features added to the part. Then someone gets the idea that the fan now can be mated/aligned to the mounting holes. But the mounting holes depend on where the fan is because that's what the user told the software - this creates a loop.

Creo will complain about the loop and many users will panic because they only "fixed" the fan that was floating and now there is a problem.

There is a tool, reference viewer, that will tell the user what the loop is but, since Creo doesn't know what takes precedence, it's up to the user, who now confused, to figure it out.

The fix is easy - go to the wall part and dimension the location and diameter of the holes there and then remove the references to the assembly. With that, no loop, as the holes no longer depend on the location of the fan which depends on the location of the holes which ...

In over 20 years of using Creo and its predecessors I had only one case where the software went wrong; that was cured with the next revision. If something has happened, it's because a user told the software to do something and if it's not what was wanted, it means that the user can certainly fix it.

An area that also catches users is they get an incorrect model in their heads of how Creo evaluates things. This is a bit odd as, at a fundamental level, Creo is stupid and that is good, because the complexity comes from clever use of a small set of functions.

For example, in family table items a basic item, such as a bolt, will be constructed of features, such as a hex extrusion for the head, maybe a revolved cut for the chamfers on the head, and either a linear or revolved extrusion for the body. Life is good. This is then converted to a family table item that adds a 2D list by adding that table.

Each row of the list get the name of each different fastener that has the mentioned features and the user can add dimensions of the features to the columns of the list to create different sizes. It looks like most any tabulated catalog page. Error number 1 - the users think the names are local to the family table so they just give a name like HB-250-100, not realizing that someone else has that same bright idea. If using a PDM (product data management) system that system will catch the problem and tell the user they cannot reuse the name. If not, then if items from both base tables are used only the one the user opened first will appear. They will look at the part they thought it was; it's now "wrong" because they aren't looking to see what table it came from.

OK. Then someone comes along and uses one of the bolts. But they realize they need to add a drilled hole for a cotterpin. So they open the part and add the hole, not noticing it is a child part (instance) of a family table part. Since the hole appears only in this part of the family table Creo adds the feature to the family table and suppresses it in the top level/generic part so, by default, it is suppressed everywhere else.

Then, here's stupid thing 2. Someone opens the generic part, notices the suppressed feature, and resumes/re-adds it. Unless that hole hits the generic part it doesn't appear. User 2 then concludes it was a mistake and deletes the feature or, since nothing happened, leaves it. Now the hole is, hit or miss, in all the parts.

User 3 comes along, finds an extra hole in one of the children parts, pulls up the child part and deletes the hole. As I recall it cannot be suppressed in the child component because it's not a feature of the child component, all features belong to the generic. So the family table now has a bunch of "YES" to the hole and some "NO" to the hole. And, for the coup d'grace, another user also needs a drilled hole, doesn't look at the generic, and adds another hole to another instance.

All of this instead of simply editing the family table to add the hole, the dimensions for the hole and then adding a properly named instance with the correct dimensions.

Were I to give an overall rule to using Creo - it's not all about you. What you do can affect everyone that has to interact with what you do. There are settings that will slow down doing damage, like locking access to family table items in the PDM so that users cannot randomly stomp on each other, or telling Creo that only local references can be made, so that the fan problem can't occur. But the Pro in Pro/E stood for Professional and the tools are both capable and very sharp and can do great things or great damage.

 

[CAD2015]

Thanks a lot, Dave!
I took notes of everything you mentioned above.
Also, thanks for the documentation link, that's going to be very useful.

Regards,

 

[dgeesaman]

I might be late to this thread but I was an instructor for CADQuest, who for years published the broadest group of Creo tutorial books out there and I think they were quite good quality too. PTC hated us because we made their training resources look bad.

I think you can learn a lot about Creo in two weeks, 80 hours. I taught a 5 day course that covered the basics of modeling, assemblies, and drawings. A more advanced user could complete the entire contents of the book, even considering the time spent listening to my brief lectures. Anyway, without the lectures an experienced user can ram through the tutorials in 3-4 days, leaving several more days to do a couple more tutorial courses such as Surfacing, Intermediate and/or Advanced modeling, Detail drafting, etc.

3D parametric* CAD has evolved and in my opinion, not for the better. When it was new, the concept of building a robust 3D model that drove the 2D drawing was universally agreed to be a good thing. Coupled with an organized Engineering data cataloging system, a designer can quickly find a similar part, make a copy, and make reasonable edits to the model and get the drawing for free or nearly free. Making that first drawing from scratch was a little slower because building a thoughtful 3D model took some time, but that is easily recouped from either time saved on revisions or reuse on later projects. Creo is really good at that if you use it sensibly, and 3DDave hit on some really important sensibilities that were rules in the past.

Somewhere in the SolidWorks/ Inventor / SolidEdge era, the focus shifted on the minimum time required to make that first drawing, and ease of revision and re-use of files has fallen as a distant consideration. Assembly components were at one time assembled in sequence, with each component being treated as a feature. It requires the designer to think a little bit, and occasionally work out things without pure parametrics driving them (e.g. the holes in the wall example - you may have needed to fully constrain the fan relative to the wall instead of drag and leave it there) and just manage having dimensions for the holes in the wall and fan separately. But then the assembly and part files are very stable and tolerant of changes to their dimensions and details. SW/Inv/SE have very few rules or chainguards to allow a user to quickly race from start to finish, making a pretty drawing in a bit less time, but also a thoroughly unmanageable mess. Creo, unfortunately, has followed suit on many of these behaviors and really undercut its core strengths in durable parametric data.

As an experienced Creo user I'm aware of where they've taken off the prior sensibility rules and not doing those things helps me avoid circular references and unpredictable regenerations. I never want to see a feature that was performed at the assembly level to show up within the standalone part. I've learned that just because a clever feature exists to make things parametric, doesn't mean it's a good choice. I urge you to learn how to make fully constrained sketches, fully constrained assemblies (ok, you don't have to lock the rotation of nuts and bolts but do constrain everything else), and learn how to construct geometry that is more tolerance of editing. Use family tables but don't get crazy.

Oh and one other thing: in the past it was safe to put a bunch of components in an assembly and add cuts and hole features to them, within the same assembly. It just regenerated starting at the top and worked down the list. At some point Creo changed the way it regenerates assemblies and mixing assembly cuts/holes with components in the same assembly file is now highly unstable. They never admitted they broke it but when you submit such a model to tech support, they'll return it to you with all of the components in a subassembly, the subassembly as the first item in the assembly, with the cuts and holes following the subassembly. Then they'll close your ticket. As a user with a wide array of assemblies made in that arrangement, that was deeply disappointing.

I used to cringe when I had to edit the Creo models made by other Creo users who did not have the deep robust Creo training that I had. But when I saw the utter insanity that was possible in SW/Inv/SE, I came to appreciate that at least it was possible to repair the Creo files. I used to assume my knowledge in SW/SE/Inv was simply too new to be good at repairing the models and re-using someone else's data but I now believe the problem is mostly that SW/Inv/SE simply don't make robust, repairable parametric content. They just force you to recreate it.

I'm going to sound old and snobby but I don't know many SW/Inv/SE users who understand how powerful good parametric models/drawings can be. They might think they know, but they're on such autopilot re-creating their drawings that I can see they don't. I see a lot of focus on using Automation in SW/Inv/SE that isn't even necessary with well built Creo models and drawings. (Fun fact: I use an automation in Inventor that makes a part & drawing. Not too complicated. It took months for a team to develop this automation and the final drawing is suitably good. The actual automation requires several minutes to execute. And yet I can manually copy, enter new parameters, regenerate, and move around dimensions in the Creo models in the same amount of time. Without any automation at all. Winning?)

PDM is indeed a whole other animal. I was fortunate to not need to use Creo in a PDM environment, and our design team was small enough it worked out just fine. I do believe that the PDM tools that support Creo might be worse than the PDM tools for SW/Inv/SE. But again, the PDM and the CAD should each earn their keep and PDM is not the focus of this.

David

 

[CAD2015]

David,

Anything you posted is very valuable and I gave it full attention.
Thanks a lot!