General transformation tool, including scale

[S_Edgenear]

As seen in a previous post, there is the lack of parametric way to scale objects. We can use an option to globally scale a part, in a non parametric way, or we could use the warp features to scale in a parametric way, but which could distort the surfaces of a model, and which does not allow to parametrically scale sketches with imported geometry, or sketches that have splines with non-dimensioned nodes.

I suggest that the "Move / Copy" general transformation tools, which currently only allow to move or rotate objects, that there should be added the option to also Scale objects, and that would also let to (move, rotate, or) scale skeches (Giving a copy of an original sketch, with the geometry scaled up or down), after picking a scale center.

Also, there should be the option to make some general transformations, using a source coordsys and a target coordsys.

Please see the attached image:

 

[StephenW]

The scale feature has been requested multiple times.

https://community.ptc.com/t5/Creo-Parametric-Ideas/Create-a-feature-on-the-model-tree-when-we-scale-...

https://community.ptc.com/t5/Creo-Parametric-Ideas/Scale-Feature/idi-p/460121

[S_Edgenear]

One of those requests was from 2012, the other from 2013... I never saw them.

[tbraxton]

@S_Edgenear 

Both items you have requested are available in Creo currently.

"...there should be the option to make some general transformations, using a source coordsys and a target coordsys."

Transforms between csys is supported in the Flexible Modeling Features. Move using constraints supports transform between two datum Csys. More detail is here but I have not seen an example of Csys transform in PTC help files. If you can not get it to work let me know and when I get time I will  provide an example.

http://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/part_modeling%2Fflexible_modeling%... 

Parametric model scaling features are available in the Mold design module. A shrinkage feature is available in mold/cast module and is a parametric feature. You can read more here.

http://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/mold_and_casting%2Fmold%2FAbout_Ap... 

[S_Edgenear]

Thank you for the reply.

a) If I'm not mistaken, Creo Flexible Modeling Features do not work in the MFG Cavity environment. At leaste it did not work in Creo 4, which we were using. I noticed we could move bodies or surfaces using flexible modeling using a CSys, but it only worked in normal part enviroment. I've not tested yet in Creo 7 if it0s already possible to do in the MFG cavity environement. Anyway, as you stated, there is no example in the documentation, and it's not so intuititive as using the copy paste functionality, even if the underlying code would be practically the same.

b) We at our company always used the shrinkage funcionality since we use the Manufacturing license module, since we are in the moulds industry. Even though I have acess to that functionality, I think it would be useful to have a standard scale transformation tool for general users. We have already needed to scale logos from imported geometry, mostly 2D geometry, and if we try to import a hundereds or thouseands of small curves or lines in the sketch environment. The scale entities in the sketch envorment distorts any splines, so, it's not functional, and using the shrinkage command in the Manufacturing module to try to parametrically scale 2D entities is not feasible either.

[tbraxton]

I can not speak to Flexible modeling within any of the mfg modules as I do not use them. That is an important context for your enhancement request, and you should make that very clear to PTC. I would suggest a couple of steps to move this forward.

1) Open a call with PTC tech support and ask for clarification on the access to FMX features within the specific module where you need it.

2) If it is not currently supported, then document a use case with enough detail to get the idea across and then submit this idea to the PTC User technical committee for the specific module where you want to see the enhancement. You can go to https://www.ptcuser.org/Committees/About-Technical-Committees  and contact the appropriate technical committee. You will have a more likely chance of getting an enhancement through the TC process than just posting here.

PTC is unlikely to implement a parametric scale feature outside of an add on module IMO. This has been a request  since the Pro/Engineer product and the answer has always been to buy the mold package.

With regard to 2D scaling of logos this is a problem that I am very familiar with. Shrinkage is of no use inside sketch mode as you noted.

The best practice in my experience is to have the logo created using a true type font which can then be referenced by the Creo sketcher when inserting the logo curves and it is scalable in sketcher. You insert text in the sketch and use the custom font which will create the logo within sketcher. I literally can type a single letter in sketcher and it will create a scalable and accurate logo. This results in a simple, scalable, and robust sketch for the logo. I have not seen a better way to deal with this specific situation.

[S_Edgenear]

I use the manufacturing module most of the time, maybe 40%, and advanced assembly and stanrard part mode the other 60%.

I understand that PTC might want to keep certain key features locked to a module, but I think that not giving a general scale option as a means to guarantee the use of the parametric shrinkage inside the manufacturing module does not make much sense. People that need the MFG module will still buy the license. Those who would not need it, they have alternatives to give the shrinkage to a part. In our work, we rarely edit the initial shrinkage value, so, most of the people that would try to save costs, could use the scale model in a non parametric way, anotate the scale value, and if later they needed to alter the final shrainkage, they would calculate a scale up or down according to the difference in scale already applied to the part. There is also a "workaround" or alternative to shrinkage, which is parametric, which is using the warp feature. It's "hidden", almost undocumented, but the funcionality is there, so, it does not make sense to not provide the same funcionality in the Copy / Paste special, which is where most users would look for a scale transformation. Still, the warp tools, which include parametric scale option, only scale solid geometry, and do not scale wireframe or sketches, which is needed for scaling logos.

I also prefere to use Text and using the appropriate font inside sketch, to model logos text, but most logos are graphic and not text based. There are logos that we have to reproduce exacly as the clients supply, we cannot re-create or simplify them. Sometimes we have to do the scaling in an external 2D program, and re-import, but if we need to change the scale, for the logo to fit at some constrained space, sometimes we have to re-import and re-project all the 2D line entites, which is time consuming.

[tbraxton]

I am not sure I conveyed how a true type font for a logo works. As an example with a custom ttf I can create a sketch with the text character "M" and then use the custom font to get this geometry in the sketch. With a single dimension I can scale this entire logo in the sketch without failures and it will maintain its aspect ratio. This approach is not limited to text characters.

[S_Edgenear]

I see what you mean, now.

By the way, which TTF Font Editor would you advise to use?

[tbraxton]

 I have never been involved in the creation of the fonts so I don't know what is used to create the font itself. The logo design is typically done in Adobe Illustrator and then converted to a font.

[S_Edgenear]

@mneumueller ,

Another use case for the option to have a scale body command, now that Creo 8 allows to have multibodies in the Mold Cavity Manufactoring environment, is to allow to give different shrinkage values to different bodies.

For instance, when making a plastic part mold, with metalic inserts, the plastic (body) will need to have a higher shrinkage value (greater scale value) than the metalic inserts. Currently there is no easy way to give parametric  different shrinkage (scale) values to different bodies or quilts. Until now we have to use assemblies and different parts, instead of different bodies to achieve this. So, there is a more complex, time consuming and error prone workaround, 

[mneumueller]

yes, forwarded it to my PM colleague for manufacturing