Synthesis Engineering
Engineering Services | Insights | Contact

Creo Workflow That Slows You Down

PTC's Creo has a lot of really nice things, but it also has some serious User Interaction burden.  In this article we will look at a few Creo Workflow examples that distract us for little or no benefit.

For each item we will display, explain, and give solutions (what we know) for these time absorbing annoyances.

These are small items, sure, perhaps distractions.  Yet they are contrary to productivity and efficiency.  Anything that takes our attention away from our work, and forces the focus on something else, makes us less productive.  So, how do we remove them, or streamline our workflow around them?

Nags, Interruptions and Unnecessary Dialog Boxes

Let's start with silly dialog boxes that nag us for stuff that doesn't matter.  These are items where Creo demands our attention, makes it look like there is a problem, or makes us feel like we did something wrong.  Unfortunately, we must deal with these Creo workflow annoyances over and over - even when NOTHING is wrong.

Mostly, these are time wasting distractions.  Here are several examples with screen shots and some Solutions.

WARNING:  Flexible Modeling!

At one point PTC was all about bragging on Flexible Modeling.  It was the star of development!  I'm not sure what happened, but now you get a WARNING if you use it.

Why is this a repeating message?  To the point, why is it warning of a problem that usually does not exist?

Creo Workflow Nag 1

Of course, a warning is good if there is a problem, but mostly, for this one, there is not.  That makes the warning meaningless because it appears when opening the drawing, not when there is a problem.  - Crying Wolf! Wolf!


- Per PTC Tech Support call CS268508,  Set the config option drawing_warn_if_flex_feature to NO to skip the warning.

- I have tried several things, but it does not go away.  So, the real solution:  PTC, please Remove it - or give us a box to check that says Don't Display Again For This Drawing."

Persistant, Obtrusive Warnings

This annoying message pops up constantly.  While it does give good information, if I'm working on a model (normal when Creo is open), I already know this.  I don't need a reminder over and over.  How do we tell Creo to stop checking?

Unnecessary Warnings

There is also a warning icon constantly in the model tree.  If there is something wrong, the warning is valuable, but when it's the same silly thing all the time, the warning becomes meaningless.  It teaches us to ignore warnings, then we will miss the important ones.


- Set the config option nmgr_outdated_mp to do_not_show then the warnings will stop.
- Note:  The PTC article CS196415, explains this and more, but it is poorly written and out of date.

Creo Model Police

How do I disable the model police?  This message insinuates it is bad to save until the model is perfect!

Creo Model Police

PTC has taught me - by sad experience - to save often or Creo will crash and loose work.  So I save often, but this ridiculous extra pop-up indicates it is bad because the default is "Cancel" - as in don't save?

If I tell it to save, I want it to SAVE, not complain.  With "Cancel" as the default, we can't just hit the Enter Key to blow by it, we must move the mouse.  This is distracting, missleading, and it slows Creo workflow.

A similar Creo nag complains about regenerating.  The solution below also addresses that, but Creo will regenerate extra every time before saving.  For small models it's quick, but with large models and complex assemblies it is a redundant waste of time.


- Set the config option mass_property_calculate to by_request to stop mass the property warnings.
- Set the config option regen_solid_before_save to yes to stop the regenerate warnings.  Note:  It will take longer to save large models.
- Please see PTC articles CS198809 and CS196808 for more information.

- I don't have a solution for the large models extra regeneration waste of time, but for me it is much faster than dealing with the redundant message waste of time.

You Did It Right, But the Creo Warning Says You Messed Up

Why is Creo complaining?  To create a thin feature, or surface, open sections are often needed, sometimes required.  Open sections are awesome in their place, so why does Creo complain?

Misleading Warning

This message is misleading, because the model often DOES have "solid geometry in the model to intersect".  And, as a WARNING, it insinuates open sections are somehow bad, which is NOT true.

Defaulting to "Surface" is also misleading.  Sure, usually there is a choice for "Surface" or "Thin", and at times we will need to change it anyway, but it does not mention "Thin" - and the wording implies "Thin" is not possible.

Furthermore, the default is "Cancel" - suggesting that the correct approach is to "Cancel" and lose your work - which is completely STUPID!  And, this default makes it so we can't blow through with the Enter Key, we must interrupt our workflow to deal with this insulting Creo pop-up.  How do we turn it off?

To PTC:  Messages like this teach customers to ignore messages.  This one is:  First, useless;  Second, misleading;  and Third, insulting (because it effectively says you don't know what you're doing).  It also tells the customer PTC is sloppy, which then disccredits other messaging.


- According to PTC Tech Support, this functions "as defined".  Aparently PTC wants you to think something is wrong.  They want to interrupt, and possibly make you lose your work.  - Fail.  The message does not even mention "Thin" features, so if that's your intent, you definately screwed up.  - Fail Again.

- PTC says this is for the new user.  But how long is a new user a new user?  And, why do you want to confuse and create problems for new users?  None of it makes sense.

Convoluted Solution:

- One way around the insult is a change in workflow for thin and surface features.  Instead of going right to the sketch, define all the other things first - surface or thin, add or remove, etc. - then sketch.  It's an alternate workflow which definitely contributes to inconsistent behavior and the slow Creo UI.

- Honestly, while it's not that big of a deal (once you understand the stupidity of the pop-up), it emphasizes again the issues that come from PTC PM's in refusing to use the product they design.  It also shows a serious lack of respect for us, the customers.

Material Units Conversion

Why would you assign a material and NOT want it to match the units of the part you are working on?  To me that seems like the rare exception, so why is it the rule?

Creo Workflow Interruption

This useless nag happens with every material assignment if the units of your materials file don't match those of the current part.  I suppose there is value in knowing it, but if you are assigning materials and know what file to assign, then this is a bit of an insult.  At least it goes away with the Enter key.

How can we tell Creo to always match the units and convert properly?


- According to PTC Tech Support, there is no way to skip this warning.  They suggest creating duplicate files for every material, one for each unit system.  That would be 3 of each material file for me to cover the common unit systems I work with.  - Fail.  That's not a reasonable solution.

Something More Like A Solution:

- Build a mapkey to assign material and answer (most of) the various dialog box nags - including both this one, and the issue below.  See the mapkey content below.

Material Assignment Superfluity

This one baffles me.  Like the PTC engineers sat around thinking of ways to add extra clicks and make the software slower.


Everytime I see this I want to scream "What did you think I meant when I told you to assign a different material?"

To understand the significance, we have to look at it in context.  To avoid the "No Material Assigned" issues, all my startparts have an "Unassigned" material with super high density.  This helps in Mass Properties calculations - part or assembly - because it is easy to see when I forget to assign a proper material.

In Pro/E, material assignment is easy with a mapkey - "SMS" (Setup > Material > Assign > Generic_Steel), and a whole bunch more.  3 keystrokes and it's done, no complaining.  You can't do it complete in Creo because there are too many warning dialogs which overlap function.  Instead, Creo wants us to jump through a bunch of time wasting hoops with every part, every time we change material.


  1. When I tell it to assign a material, why does Creo interrupt the workflow by questioning what I just told it to do?  See the "Material Units Conversion" above for an example.
  2. Is there a way to tell Creo that when I assign a material, make it the "Master"?  The extra steps each time are unnecessary.  For good UI, it is far better to manually set exceptions, than to require extra steps every time.


- According to PTC Tech Support, there is no way to skip the warnings.  To avoid this pop-up you can delete the existing material first (as extra steps with different pop-ups).  - Fail..

Something More Like A Solution:

- Mapkeys will do some, but not all.  So, build a mapkey that answers most of the nags.  The code below works in Creo for a material in the pro_material_dir named steel_generic.mat.  It works if another material is assigned, or if no material is assigned.

mapkey(continued) ~ Select `finder` `FFileListPHLay.Filelist` 1 `steel_generic.mat`;\
mapkey(continued) ~ Activate `finder` `FFileListPHLay.Filelist` 1 `steel_generic.mat`;\
mapkey(continued) ~ Activate `UI Message Dialog` `yes`;\
mapkey(continued) ~ RButtonArm `finder` `FModelList` `STEEL_GENERIC`;\
mapkey(continued) ~ PopupOver `finder` `InModelPopup` 1 `FModelList`;\
mapkey(continued) ~ Open `finder` `InModelPopup`; ~ Close `finder` `InModelPopup`;\
mapkey(continued) ~ Activate `finder` `FAssignPushPopup`;\
mapkey(continued) ~ Activate `UI Message Dialog` `ok`; ~ Activate `finder` `FOkPush`;

You can easily copy the mapkey for a material of your choice by changing the filename in 3 places.  You can expand the use for many materials - like SMA for aluminum, and more.

Unfortunately, because of the numerous warnings and insults, I did not find a way to make it work everytime, like when the material is already in the list.  In older Pro/E it was smart enough to know, and ignore it, if you tried to assign a material twice.  (Helpful to type the mapkey again if not sure about the material assignment.  Type and it's sure, no complaints.)  Now, with Creo's degraded functionality, you are punished with extra warnings and dialog boxes if you happen to type the mapkey a second time (even if it is days later).

PTC PM's obviously did not think thoroughly before adding this.  But, they don't use the software, so how could they know?  So much for all the bragging (lies) about speed and efficiency.

Enough For Now

Thank you for visiting.  Hopefully this will help as you deal with Creo popups that interrupt workflow.

Articles For Working Through Creo

Thank you for reading.  If you agree with any of this, please contact PTC and let them know we expect better quality in the software, not just with the bugs, but in the User Interface too.

In the meantime, here is the list of Creo articles to read.  Good luck with all your Creo Design.

- PTC's Creo: Awesome CAD Power, Mired In User Interface Woes
- Learning Creo? - Start With The Paradigms
- Creo Workflow That Slows You Down
- Coming soon:  Drawing 'How To' - Selection Frustration.

Stay tuned.  There is so much more to come!

Synthesis Engineering Services, Inc.
Always Innovative Product Development & Functional Engineering Consulting!

Copyright 1995-2024