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

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.

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 ...

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

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 ...

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!

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),

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).

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)

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

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.

Add me to the long list of users who are incredible frustrated by this de-hancement. Our company leapfrogged from Creo 8 to Creo 10, so I'm late to the party, but this change is positively horrible. We have lost some fundamental functionality in project and offset in sketcher. Losing the ability to select a surface to project or offset a loop, and losing the ability manipulate individual segments of project/offset of full or partial loops, has made the tool less useful and the workflow less efficient.

I've been a regular user of Pro/E / Creo since 1990 (Pro/Engineer Rev 5). This is the single biggest UX blunder I have experienced in any update over all those years. Please listen to your users and fix this! I'm right now trying to figure out how to get an authorization code to allow deprecated config and enable the SKETCHER_USE_CREO8_PROJ_OFFSET config option.