With the new Offset tool, is Convert to Tapered functionality lost?

[Pettersson]

I like the new (well, it's been a few years now) tools for Project and Offset. They're harder to teach, but they're more robust. But today I tried to use a seldom used command: Convert to Tapered. It used to be you can select an Offset geometry in the Sketcher and hit Operations->Convert to->Tapered, and then have the offset vary from one end to the other. Nice little trick.

Well, it seems it doesn't work anymore? I tried getting it to work, but it's always greyed out. I searched through the documentation, and found this little note: 

When you use the new tools for offsetting or projecting an edge the following functionality is not supported.

• Projecting an axis.

• Projecting or offsetting in the Blend tool.

• Creating a Pattern of the type Curve.

• Converting the new offset geometry to Tapered.

Hm, I guess we got some new limitations with the new tools. But the fact that the option is still there (but greyed out) and the fact that the documentation says when you use the new tools leads me to think that there is perhaps a way to use the old tools? I looked through the options, but couldn't find anything. Is it possible to make a tapered offset in newer version of Creo, or has that ability been removed (in which case, why is it still in the interface?)? Does anyone know?

[tbraxton · Accepted solution]

There is a hidden configuration option available to use the legacy offset functions in sketcher. Add this line to your config.pro file to use the old offset functionality. Note that you will need to set this option to "NO" in order to invoke the new version in the same session of Creo if this config option is loaded as set to "YES".

SKETCHER_USE_CREO8_PROJ_OFFSET YES

[Pettersson]

Thanks, what a classic!

"How do I do X in Creo?"

"Well, first you need to go into the config and activate this secret command ..."

It's not the first time. 😀

EDIT: Seems like it's a deprecated option, meaning to use it I'd have to get permission from PTC. I guess the Convert to Tapered function should be considered lost for all practical purposes. A pity! Not sure if there is a good workaround?

[tbraxton]

There is a reason that the config option is a hidden one. There has been a lot of user pushback on PTC regarding the new sketcher offset functionality and the inability to deal with scenarios where the old version simply works or works better. Credit is due to PTC for creating this config option after deploying the new functionality so that users can revert to the previous implementation.

[KenFarley]

Wait, does this mean if I set this option I will be able to offset lines and arcs, as a chain, instead of having to do much more extra geometry creation? That would be really nice. When we switched to Creo 9 from 4, the first time I experience this "de-hancement", it triggered a lengthy diatribe on here (by me). It was a big boot to the neck, to be sure.

[tbraxton]

With the option set to yes, the UI /functionality reverts to the Creo 8 version of the offset tools.

[Pettersson]

There are some inconveniences of the newer Offset and Project tool, to be sure, but overall I think it’s an improvement, as it enables the user to use smart chain selection techniques to create more robust references rather than referencing each curve individually. It would have been even nicer with a toggle button to choose whether to offset as a chain or as individual entities, especially since some functionality was lost (like the Convert to tapered operation).

[ByDesign]

I don't know about Creo 8 (or earlier), but in Pro/E you could offset a chain of curves, and you could convert the whole string to tapered.  How else can you even perform such a function accurately?  Especially with a series of splines or conics?  Moreover, where are you supposed to learn about "Hidden" options if you don't get lucky in some google search?  I think this is customer abuse.

I will say, I like your idea of a toggle if they are not smart enough to find an elegant solution.

[ByDesign]

Seriously?!?!  "Credit due to PTC"  for removing great functionality? . . . "Credit due" for dumbing down the software?  For putting a band-aid on their mistakes?  For assuming the customers are too dumb to use the awesome functions we have had for years?

More like let's take them out behind the woodshed for an attitude adjustment.  The biggest problem in all of this is the people making the decisions are not actually using the software - like really using it - so they don't understand the value of what is/was there, nor the consequences of their ignorance.

I used to compare great things PTC software would do that others could not.  Now I look back longingly at functions Pro/E did that Creo cannot.

[tbraxton]

1) PTC deployed the config option after users identified deficits in the new offset tool. They listened to the users and reviewed the arguments resulting in the creation of the config option. The development and deployment of the new functionality would have surely benefitted from super user feedback to PTC, but they did implement a "patch" for this issue. I for one am glad that they did!

2) The convert to taper is still available. Here is an example of a tapered offset in Creo 10.

[ByDesign]

Convert to Taper is grayed out here.  Is there a magic trick to do it with a chain?  Pro/E did it.

[tbraxton]

Use the config option shown in the marked solution in this thread to access the "old" functionality which is what you are asking for to use taper.

[ByDesign]

That is the current state - as noted by the single entity with a tapered offset.  I have actually tried it with hidden config option both YES and NO.  The screen shot above has the option set to yes.  The offset was created using "Chain".  I also tried it as "Loop" but it is the same.  "Tapered" remains grayed out if I select anything other than a single entity for offset.

[ByDesign]

I suppose I could try combining entities into a spline in a second almost identical sketch to the original, but I have not had good luck with those unless the entities are tangent.  Also, I need the base entities later, so that would mean multiple duplicate sketches which create problems downstream.  I'll try it but it looks like a disaster in the making.

[ByDesign]

@tbraxton So I guess you can eventually get an approximation if you do it in several steps, duplicating sketches, putting in radii where you don't want them, creating a spline, then in yet another sketch create the tapered offset.  It won't combine the curves if they are not tangent.  There was an "exact" combining function in Pro/E, but I can't find that in Creo.

I say approximation because the next step after what you see in this screenshot is to build yet another sketch with the arcs back to sharp corners referencing the geometry of this offset spline.  That will be hard to make it update properly with dimension changes.

This is a ridiculous workflow all because some PTC PM couldn't figure out that there must have been a reason for putting the functionality in there in the first place.  Obviously they don't use the software they define.

[RandyJones]

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@ByDesign wrote:

@tbraxton So I guess you can eventually get an approximation if you do it in several steps, duplicating sketches, putting in radii where you don't want them, creating a spline, then in yet another sketch create the tapered offset.  It won't combine the curves if they are not tangent.  There was an "exact" combining function in Pro/E, but I can't find that in Creo.

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The Exact and Approximate copied curve types is still there:

https://support.ptc.com/help/creo/creo_pma/r12/usascii/#page/part_modeling/part_modeling/To_Copy_Curves_and_or_Edges.html#

[ByDesign]

@RandyJones  That is interesting.  Thank you for pointing me to that function.  It turned the sketch into a curve, but did not combine the entities.

For this case with tapered offset, it does nothing because it maintains the individual elements - like the original sketch.  So, it is a nice thought, but unfortunately does not help with the tapered offset.  Thanks again for the input.