Learning PTC Creo.......... 1

[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,