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Problems with the "Modernized Project/Offset Tools" in Sketcher of Creo 9.0.0.0

bmancini
13-Aquamarine

Problems with the "Modernized Project/Offset Tools" in Sketcher of Creo 9.0.0.0

Hi,

I have several problems with the Modernized Project/Offset Tools in Sketcher of Creo 9.0.0.0.

I wish I could go back to the old command present in creo 8.0...
I explain what the problems are:

 

PROBLEM 1:

In creo 9.0.0.0 the project / offset tool does not generate the arc centers of a loop.

bmancini_0-1658146798118.png

 

bmancini_1-1658146805166.png

 

PROBLEM 2:
After using the command I would like to be able to select specific segments and arcs generated with the Project / Offset command and then perhaps mirror them, but with the new command it is no longer possible ... all entities are selected as a group, is there a way to explode them?

 

PROBLEM 3:

The "Delete Segment" command is NOT ABLE to recognize the segments defined by a project / offset loop of a curve with intersections on the segments and references.

P.S. Notice the yellow dots that delimit the recognized segments.

bmancini_3-1658147087783.png

bmancini_4-1658147188769.png

 

PROBLEM 4:

I would like my arc to have the same radius value as the arc of the offset chain, but the program does not allow me to set the constraint because it sees the entities of the offset chain as "a single group entity".

bmancini_0-1658148293918.png

 

I am really disappointed with the command, I think it is intolerable.

I have watched all the official videos on using the command, but still I cannot appreciate this new version of the tool.

Does anyone know if it was possible to reactivate the old command?

I'm curious how you feel with the new command.
Thank you.

 

19 REPLIES 19
tbraxton
21-Topaz II
(To:bmancini)

Reverting to the "old" command  is not supported in Creo 9.

 

The documentation indicates the ability to switch between chain selection to one-by-one.

"Switching from rule-based definition to individually selected items is supported for “Project”-tool"

 

Have you tested the method presented here? 

https://www.ptc.com/en/support/article/CS369555 

 

If it does not work then you need to open a call with support. If you log a call and an SPR is generated, please post that information in this thread.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
bmancini
13-Aquamarine
(To:tbraxton)

Thanks tbraxton for the reply,
I read the articles:
https://www.ptc.com/en/support/article/CS369555
and
https://www.ptc.com/en/support/article/CS369607.
What they propose in the CS369555 to convert the chain to one-by-one for the "Project" tool may be reasonable, but I still don't like it.
What they propose in the CS369607 to convert the chain to one-by-one for the "Project / offset" tool with the "thickness" tool is unreasonable because, in my experience, the tool inevitably creates a double entity profile forcing the operator to select one by one all the entities of the second useless profile.


Can anyone tell me if it is possible to obtain only one offset profile with the "thickness" tool?


I continue to be very frustrated and disappointed.


@bmancini wrote:

Thanks tbraxton for the reply,
I read the articles:
https://www.ptc.com/en/support/article/CS369555
and
https://www.ptc.com/en/support/article/CS369607.
What they propose in the CS369555 to convert the chain to one-by-one for the "Project" tool may be reasonable, but I still don't like it.
What they propose in the CS369607 to convert the chain to one-by-one for the "Project / offset" tool with the "thickness" tool is unreasonable because, in my experience, the tool inevitably creates a double entity profile forcing the operator to select one by one all the entities of the second useless profile.


Can anyone tell me if it is possible to obtain only one offset profile with the "thickness" tool?


I continue to be very frustrated and disappointed.


Hi,

I think the best way how to get the answer is contacting PTC Support.


Martin Hanák

The articles 369555 and 369607 have been updated. We hope that gives more background to the reasons and intent of the changed behavior and the recommended workflows.

R&D is continuing to research potential further refinements to the new workflow for future releases.

In addition, we currently plan to add the "All-curves-in-feature" rule to the chain collection workflow in Creo 9.0.2 which was not included in the initial implementation in Creo 9.0

 

bmancini
13-Aquamarine
(To:mneumueller)

Thanks Mneumueller for the update.
I hope the situation improves soon.
I wish you good work.

Bumping this up and encouraging all to go and vote on the submitted product idea and voicing your opinion about this situation.  Though it is stories such as these that make me think that the "product ideas" part of this community is a bit of a waste of user's time and it has become more of an end process for PTC when resolving support cases: 1) customer points out a problem and opens a support case; 2) customer is told "software works to specification", so they are asked to file a product improvement idea; 3) case closed; customer feels better, thinking something will be done.

 

It's rather brilliant - PTC gets a well documented report of a deficiency (for free), the to-do list is automatically updated, and if and when they feel like it, R&D will work on it sometime.

 

The implementation of the "improved project/offset tools" is disappointing, (perhaps in part due to lack of end-user testing and feedback): PTC removes the user-liked functionality and arguably, does not fundamentally add anything new - because the option of constructing composite curves and using them for projecting in the sketch was already available.

 

Circling back to product ideas: I'm curious why R&D worked on "improving" the project / offset tools in the sketch?  The articles tout the benefits of standardized workflow, sketch stability, reduction in the number of references to manage, etc...  That's arguably all real and valid, but my point is that I don't recall one product idea in which a customer asked for this "improvement" and started the ball rolling.  But then again, I probably missed it - among countless user ideas that have been ignored by PTC... for decades.

bmancini
13-Aquamarine
(To:bmancini)

Reporting other anomaly:
PROBLEM 5:

If in the sheet metal environment I try to close an opening with the "Wall" command, and then use the project to detect the profile, the feature goes into error ...

bmancini_2-1663054937318.png

bmancini_3-1663055017887.png

If I draw the outline without using the projection, it works!

bmancini_4-1663055161635.png

 

 

 

 

Dear bmancnini,

thank you for your additional report #5, even though I don't think it is related to this topic/thread of modernized Project tool. as it seems this is a behavior also seen in previous versions. Actually when I quickly tried it now, I only saw it in prev versions and I couldn't reproduce it in Creo 9.0 anymore.

Therefore, I would encourage you to report a SPR to Technical Support along with the problematic Creo 9.0 example, so that R&D can have a look at it.


Meanwhile here some alternative workflows using parametric regeneration of the loop that worked for me. You can try them out:

a) Use the "Remove Feature" on the "Loop Surfaces" (by specifying the surface and an edge of the inner contour). 
or
b) Use the planar wall feature referencing an external sketch containing the projected geometry
or

c) Use the planar wall feature with an internal sketch and projected entities as in your example, but check the Planar Wall feature option "Do not merge to model". Then use the separate "Merge Wall" feature to merge in a second step

 

best regards

 

I got a small update from R&D: a fix for this went into Creo 9.0.1.0 

bmancini
13-Aquamarine
(To:bmancini)

PROBLEM 6:

Other anomaly ...
if in a sketch, I mirror a geometry generated with the loop project, the program is not able to maintain the dimensional constraints of the parent geometry ...

 

bmancini_0-1663080423251.png

 

 

Thanks - will check with R&D

Aaron_Daniel
13-Aquamarine
(To:bmancini)

In the past PTC has often included an option in the config file to use a new method or retain the old method - they should have done that with this workflow change.  Not only does the new method require additional mouse activity and clicks, it's not reasonably intuitive to implement, and it eliminated previous selection capabilities.  

 

Prior to the "Modernized Project/Offset Tool"...

When using 'Project' within Sketcher, when set to 'LOOP', a prior sketch could be selected, and all of the prior sketch's elements would be created.


This ability is gone in Creo 9.0.

One ability that I have desired of 'Project' and 'Offset' is to pick a surface, and have all the surface edges selected (holes, cuts, or protrusions).  If I have a boiler tube sheet with many holes, I might want to select all but two or three of the holes in a new sketch.  As it has always been in Creo, I have to select the edges of maybe 40 of 43 holes...rather than select all of the holes in the sheet, and then "de-select" the three that I don't need - very counter-productive.

For reference see:  Projecting Curves or Edges in Sketcher - PTC Community<https://community.ptc.com/t5/Creo-Parametric-Ideas/Projecting-Curves-or-Edges-in-Sketcher/idi-p/727309>

There should be a way to select a surface and create sketcher entities of every edge.

 

The new "Modernized Project/Offset Tool" could be improved by adding some enhancements as described below

A) In the Chain>References>Rule-based window –add a ‘Rule:’ button for “All Surface Loops”.

B) In the Chain>References>Rule-based window –add a ‘Rule:’ button for “Selected Sketch/s”. (This would add the capability available in previous Creo versions as described above).

C) Somewhere in the selection process there needs to be a button to select if the selection chain is treated as a complete inclusive chain, or as individual sketch entities.

D) Make it so that exiting the reference selection process automatically selects all that has been selected and creates the sketcher elements – instead of having to select a button (losing all the elements if not selected) to exit the process.

 

E) In the Chain>References>Rule-based window –add button to remember all the current selection options.

 

Again, there should have been a config option to keep the old method, or use the new method (so that those who wished to struggle through the new implementation could contribute to its refinement till it is actually beneficial).  The new method has some interesting possibilities in terms of "Intent" (so that changes to geometry prior to a sketch do no not cause unnecessary failures or unpredictable results...so it could be a good way to go...with some refinements.  Until that happens, the new method is an irritating frustrating time-trap!

it is correct that we do consider these adoption options when we do significant changes, but there are implementations where this is not feasible due to incompatibility and other reasons as in this case. To a certain extend, the currently available capability to switch to individual entities should somewhat represent a way to get close to the previous behavior (at least for project)

We did include this capability in the beta testing, but unfortunately the problematic aspects had not been raised at that time. 

R&D is investigating how to refine the workflows to provide combined benefits of previous and new behaviors for the various use cases. For example - as mentioned in the article - Creo 9.0.2 includes the "all curves in feature" option, which will address some of your points. 

 

Addition: Please see update at:   Fix Modernized Project and Offset Tools in Sketche... - PTC Community

And if you are interested in joining our review, just le me know as indiciated.

bmancini
13-Aquamarine
(To:bmancini)

PROBLEM 7:
Usually with Creo 8.0 to create a counterbore slot for screw, I used the project offset command, then I deleted the relative offset dimension (Picture 1),

bmancini_0-1664792310577.png

the program converted the "edge offset" constraints into coincidence constraints, tangency and horizontality and finally I added a dimension to the diameter of an arc of the slot, work completed (Picture 2).

bmancini_1-1664792336186.png

Now in Creo 9.0.0.0 I am no longer able to perform these steps.
When I delete the offset value, the program converts the only offset constraint of the complete or partial loop (picture 3)

bmancini_2-1664792355988.png

into tangent and horizontal constraints but not coincident in the centers of the arcs ... (Picture 4).

bmancini_3-1664792373385.png

This behavior is partly attributable to other unwanted behaviors that I have already reported in other points of this discussion, but I wanted to report it anyway because, for me it is a basic use of the project offset command.

tbraxton
21-Topaz II
(To:bmancini)

Keep posting the use cases where the new tool is not better or incapable of the same results as the previous implementation. It is the best way to get a resolution implemented. If you have not done so yet, I would open a support case for these issues. Once an SPR is assigned then it is tracked internally at PTC.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

Hi,

please replay video diameter_dim.mp4 related to PROBLEM 7.


Martin Hanák
bmancini
13-Aquamarine
(To:MartinHanak)

Hi Martin,
thanks for the video, having preached the diameters of the buttonhole is a procedure, which although more elaborate than it was in Creo 8.0, that works! Good job!
I'm curious, have you experienced it personally or have you found it in some other discussion, I tried to look for other discussions but without success.

Hi,

I just tested if problem 7 is related to sketch reference selection. And I was lucky to hit it.


Martin Hanák
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