Fix Modernized Project and Offset Tools in Sketcher

[idrive101]

1. Describe your environment: What is your industry? What is your role in your organization? Describe your stakeholders.
Product design studio, I'm a senior designer.

2. What version of Creo Parametric are you currently running?
9.0.1.0

3. Describe the problem you are trying to solve. Please include detailed documentation such as screenshots, images or video.
The Modernized Project and Offset Tools in Sketcher is proving to be very time-consuming as it adds many clicks to perform operation that used to be very fast.

Projecting or Offsetting a loop until Creo 8 used to require 2 clicks to select the command and Loop, then 1 click per loop. Now in Creo 9 it takes 4 clicks to set up, 1 click per loop plus 1 click to confirm each loop.

And, each loop is treated as a single entity where I cannot delete one or more segments of it using Delete segment, which again adds the time-consuming operation of deleting the loop and re-Projecting it as a partial loop.

I understand you're trying to improve this command, but I think you should take a better look at all the possible usage scenarios before implementing such a big change.

4. What is the use case for your organization?
The new Sketcher features are proving to be unnecessarily time-consuming, our work takes longer with no apparent benefit.

5. What business value would your suggestion represent for your organization?
It would make work lighter and faster.

[StephenW]

There is a post in the forum about this problem and the product manager has commented on that post.

https://community.ptc.com/t5/3D-Part-Assembly-Design/Problems-with-the-quot-Modernized-Project-Offset-Tools-quot-in/m-p/807476

[TomU]

Is it really an improvement if it takes more clicks and is more difficult to reach the same end condition?  Seems like a lot more testing should have been done by actual end users before this change went into production.

[olivierlp]

Thank you @idrive101 for your idea. Based on the information you provided, we are acknowledging it as the Community management team. This is not a commitment from the Product team. Other users may comment and vote your idea up.

[idrive101]

The "imrovements" made to the Project and Offset commands in Sketcher are proving very time-consuming.

Look at the videos: the same file, I need to project a series of multiple lines.

In Creo 7 (or 8 ) it takes 20 seconds, in Creo 9 over a minute. And, if at the end of the Creo 9 video I clicked on OK to close the sketch and proced to Extrue I would have lost all of it because I forgot to confirm the Project command first.

Note: I know I can just select the sketch and Extrude it, I did it this way to simulate the issue and prove my point 🙂

Here is Creo 7

And here Creo 9

We use Project/Offset a lot in our workflow, on a 3-week project the additional time it takes to perform these actions can add 1 day to the total time.

Why can't I select single/partial/loop before I start projecting?

Why do I need to confirm after projecting each loop?

Currently if I confirm using the middle mouse button I exit the Project tool.

Maybe clicking confirm once could confirm the loop, and a second click to confirm/exit Project.

[idrive101]

PTC Support told me to "make my case" about this issue by opening a new Idea along with videos (they're working for me) to prove the issue and the actual idea on how to fix it

[StephenW]

@idrive101 

PTC support always says "make a new idea" but in reality, there may already be an existing enhancement request (Idea).

I asked because the other one already has votes and refers to this post https://community.ptc.com/t5/3D-Part-Assembly-Design/Problems-with-the-quot-Modernized-Project-Offset-Tools-quot-in/m-p/807476 which has a lot more explanation and had gotten the attention of the PTC product manager who is responsible. 

Also, the video's now work for me. I think I had come across the post too quick and they hadn't finished processing.

[S_Edgenear]

I like the new modernized Project and Offset Sketch in Creo 9, and I can see why it where needed. In this case, the user is projecting from an existing wireframe (Datum curves or sketches), which takes more time than in the previous Creo versions. But if the user is projecting loop edges  of existing surfaces (which we do a lot more time than projecting from wireframe geometry), than the new methodology greatly speeds things up, no need to have to constantly click "Next" to select a specific edge loop withing a surface which could have dozens of internal loops. In Creo 9 the user can click a specific loop even if the surface has hundreds of internal loops, which saves much time clicking. So, the best thing is for to PTC to not discard the new Project enancements when projecting from surfaces, but try to combine of mix with the old methology when projecting wireframe geometry, allowing direct clicks and no need for confirmation for each project action.

[CA_10146793]

I was able to simulate the "old way" by applying a mapkey to the "new way".  It's kind of a cheap approach but it seems to work:

FIRST MAPKEY:

mapkey ueo @MAPKEY_LABELUse Edge One-by-One;~ Command `ProCmdSketProject` 1;\
mapkey(continued) @PAUSE_FOR_SCREEN_PICK;~ Activate `Odui_Dlg_01` `stdbtn_4`;\

SECOND MAPKEY:

mapkey uel @MAPKEY_LABELUse Edge Loop;~ Command `ProCmdSketProject` 1;\
mapkey(continued) ~ Trigger `Odui_Dlg_01` `t1.chn_coll_rep_list` `0`;\
mapkey(continued) ~ Trigger `Odui_Dlg_01` `t1.chn_coll_rep_list` ``;@PAUSE_FOR_SCREEN_PICK;\
mapkey(continued) ~ Activate `Odui_Dlg_01` `t1.chn_coll_dtl_pb`;\
mapkey(continued) ~ Select `chain_dlg` `ChainMethod` 1 `others`;\
mapkey(continued) ~ Trigger `chain_dlg` `AnchorLst` `0`;~ Trigger `chain_dlg` `AnchorLst` ``;\
mapkey(continued) ~ Select `chain_dlg` `RuleOptions` 1 `loop`;\
mapkey(continued) ~ Activate `chain_dlg` `OKButton`;~ Activate `Odui_Dlg_01` `stdbtn_4`;\

Press enter in notepad after the last backslash of the mapkey text.  Then for each mapkey,  select the "mapkey(continued)" lines including the blank line.  Copy to the clipboard and paste a bunch of times in rapid-fire succession.  Remove the last backslash to end the mapkey.

[mneumueller]

Hi all,

#1) Please find below a video illustrating and commenting on aspects of the workflow in Creo 9.0 as well as an enhancement in Creo 9.0.2 that further accelerates the workflow.

#2) In addition, we plan a meeting to review further refinements of the project/offset workflow that are currently in work for Creo 10.0.  If you are interested to join (it will likely be in 4-6 weeks from now), just send an e-mail to mneumueller@ptc.com   with the subject "Project/Offset Review".

We are looking forward to your participation

[CA_10146793]

Thank you for sharing, mneumueller. 

The "all curves in feature" is obviously a powerful option that users will welcome.  Additionally it would be great if the development team could consider ways to simplify these combination-click selection operations (e.g. click/shift/RMB/click another spot) where it makes sense.  I realize that PTC appears to be trying to standardize, but in some cases it amounts to a lot of excessive clicking.  It looks fast in the example above, but requires a lot of focus and mouse clicking to get it done that fast without screwing it up at least once.   Consider the case of a 2d sketch filled with multiple loops, and you want to grab a number of full loops (but not all) - this multi-step selection process may make your brain hurt.  At that point the selection process is unnecessarily complicated and further away from the intuitive realm. It would be a lot easier and more intuitive to have a pop-up window appear at the beginning of the tool with the various selection processes, and then give the user the ability to "pin" the selection option down before clicking.  That way you could simply click once on single entities to select each loop.  This is of course the more "traditional" way of selecting entities in CAD, but it makes more sense in some cases.

[idrive101]

@mneumueller, thank you for the update. From the video it seems much faster than before, and the ability to cycle through the options rather than opening the selection rules window sure is an enhancement.

I'm downloading version 9.0.2 and I'll try it out today. I'm also sending you an eMail for the Creo 10 review meeting.

One more thing that could improve this command would be the ability to swap the refecence mode between Loop and Single lines.

I don't know if I should open a new Idea or just keep adding here.

The scenario is this:

Last week I projected/offfset some lines as a Loop. Creo interprets the loop as a single line even though it is made up of many segments (lines, arcs, splines, whatever).

Today I need to modify the sketch and only keep a portion of the projected Loop. I draw new lines and I need to Corner trim the new lines with some lines form the loop, but it doesn't work because the loop is a single line, single reference.

I should go back in time and project the lines as single items, which sadly is impossible, so all I can do now is delete the loop and re-project just the portion I need.

Solution idea: an Explode command, which eplodes the single reference into a multiple-lines reference.

[mneumueller]

Thanks for the comment, CA_10146793

Please note that I would expect that your example could be easily addressed by projecting all curves into the sketch and then removing those you don't want (for example using box selection which is available once you have the projections within the sketch environment).

[mneumueller]

Thanks for the comment, @idrive101 

If I understand you correctly, then I think both suggested workflows already exist.

Once you have a complete loop projected into your sketch, such as the "C" in the previous example, then you can do the following:

a) double click the loop entity to open the chain selection widget

b) click on the details button

c) either switch to partial loop to (re-)fine start and end segments of your chain or switch to "Standard" to convert the selection into individual entities

Is that what you where after?

[idrive101]

@mneumueller 

I tried what you wrote in version 9.0.1 but I'm not getting the result I intended.

I double ckick on the loop, select Standard since I want each segment to have its own reference, but when I click Confirm only one segment remains.

Maybe I'm doing something wrong? (see video below)

And, even if it worked as intended, if it could ideally be done by pushing a single button (or right-click and pick Break-up references) would be even better.

[mneumueller]

Creo 10.0 further enhances the project/offset workflows to combine benefits of the previous and new approach. See

Broadened Support for Modernized Project and Offset Tools in Sketcher (ptc.com)

[jschneider]

As a 29 year user, I see the new "Modernized Project and Offset Tools in Sketcher" as two steps BACKWARDS

I often want to offset a chain/loop and then modify the resulting sketch.  The functionality is no longer available.

[idrive101]

I finally had a chance to use the "improved" Project and Offset in Creo 10.

I still see some issues, and as @jschneider wrote I still end up taking longer than in Creo 8 (or earlier) to perform the same tasks.

A. I can't project/offset more than 1 loop at a time. I select the loop of curves then I have to Accept, then select the project/offset command again.

B. The projected/offset items are diffcult to manage or modify, and if I remove some segments the resulting lines are marked as not closed. See the attached video. I tried Corner to join the ends of those curves and it didn't work, I have to move one of the vertexes and the use Concide. Not the most efficient way to work and, honestly, it's quite disappointing.

[mneumueller]

wrt to A: 

did you use the "repeat" button highlighted in blue below?

wrt to B:

thanks for raising it. Could you please file a Tech Support case for this so it can be looked into? 
Thank you very much.

[CA_10146793]

I agree that the ability to "pin" a loop selection is missing.  As a workaround, I created a mapkey for "use edge loop" and "offset edge loop" that enters the loop selection dialogue immediately after selecting the first entity, then pauses to allow selection of the surface loop reference.  Then I use my universal mapkey for "resume mapkey" (RES, that I can trigger very quickly with my left hand on the keyboard) to accept selection.  I copy/pasted the mapkey content 10 times in config.pro to automatically retrigger the original mapkey after every loop selection.  It's not quite as fast as the old way of picking new loops one click at a time but much faster than repeatedly mouse clicking through the menus.

[gcambiaghi]

I hope very much that this new feature will be revised because it is really absurd to use it, it is from 1993 and back in the days it was difficult to use it but this new feature besides being wasteful in terms of use the composite curve is useless, on the offset you cannot convert to standard, in project you can but the radii become spline.... and this is another absurd thing.