CREO 10 variable names and variable arithmetic in SKETCHING

[cgherghe-2]

This is a new sketch, not a part.
I want to rename the two dimensions to x = 15 and y = 20, and use, for all my dimensions, mathematical operations on x and y (instead of calculating and typing in numerical values), as follows...

For horizontal dimensions x1 = 5x/7 and for vertical dimensions y1 = 3y/5, and maybe down the road x5 = 2*x3 and y7 = y2/4.

Is this possible in CREO 10, and is it possible for a part as well as a sketch?

I cannot find anything of that nature in the sketcher, right clicking on a dimension in CREO 10 does NOT bring up the DIMENSION PROPERTIES window.

Apparently the DIMENSION PROPERTIES window does not exist in CREO 10 sketching anymore.

Would the normal mathematical operators be used and what would be the correct syntax, for both naming and using the names in the subsequent operations?
Like + - * / (addition subtraction multiplication division) and so forth...

[tbraxton]

It would seem you are asking about sketcher relations, although that is not explicitly stated in your query. As a general rule one should not use sketch relations except for the use of trajpar parameter (variable section sweep features) where the relation must be defined in the sketch for the sweep section. There are some rare exceptions to this rule of course, however your stated goal would not lead me to recommend using sketcher relations to capture the design intent you have documented here. There is no need to rename the dimensions as you can control their values using relations and parameters.

About Relations

About Notebooks

To accomplish what you seek to do you can use a notebook to define global parameters and relations using the parameters which can then be declared to any model as required. You can also save the 2D sketch for re-use in a feature as needed.

In a notebook (.lay file type) assign values to parameters X & Y and then add the relations for X1 and Y1 as a function of X&Y. You would then either import the sketch or create it in a model and then declare the notebook to the model. You can now use the relations in the notebook in your model to drive the feature dimensions analogous to those shown in your sketch above.

[Radovan_DT]

Just use switch dimension and instead of x and y, you need to use the dimension ID

sd1=15
sd0=20
sd4 = (sd1*5)/7
sd2 = (3*sd0)/5

And when putting in new dimension just insert the mathematical formula, and then the sketch will be parametric no matter if you scale it up or no.

[tbraxton]

I would strongly advise against implementing this as @Radovan_DT is suggesting here. His solution will work but it will potentially cause you headaches in the future when working with models that use sketcher relations. Only use sketcher relations if you understand the limitations of them.

Since you are asking how to control a sketch parametrically, I assume you would save this sketch for reuse. If that is the case, then you should consider how this sketch would be used in new models. If the sketch would only ever be dependent on references and parameters defined within the sketch (unlikely in practice) then it might make sense to sue sketch relations. If not, then I would definitely not use sketch relations to control any of the dimensions in such a sketch.

Searching for sketcher relations is not supported in Creo (using search tool). If you do use sketcher relations it would be a good idea to place comment lines in the model relations documenting what is done in the sketches in case someone needs to debug anything defined in sketcher relations.

Creo supports relations in a model at various levels such as - assembly, part, feature, section. Without a complete understanding of the design intent, you need in your specific application I would suggest that you use feature or part parameters to control the dimensions you presented in your post. If you provide more detail on how these relations are to be used to control your designs, then you will get more relevant options back from the community.

Article - CS336390 - Is there a report to display all relations in a model at any level - assembly, skeleton, part, component, feature, inherited, section, patterns, solid weld etc?

[cgherghe-2]

Let me understand this, will the problem be generated from the interpretation of that first 15 and 20 that show up as the values of those first variables? 

[tbraxton]

@cgherghe-2  I am not able to answer your question about a problem being generated as there is not enough context given by you regarding the design intent you need to capture in Creo. If you explain how you intend to use the variables x,y and the calculations given as:

x1 = 5x/7 and for vertical dimensions y1 = 3y/5, and maybe down the road x5 = 2*x3 and y7 = y2/4

As examples here are two possible scenarios (if they are not representative then reply with details on what you need):

Can you confirm that you are creating this sketch to save for reuse in your workflow to create new parts by importing the section into a model?

Do you need to create a feature within a single part design that you can modify using the above functions?

If you detail how this sketch is used in your workflow for design, then we can offer some options for how to best capture within Creo the design intent.

[vnamboodheri]

Hello @cgherghe-2, 

It looks like you have some responses from some community members. If any of these replies helped you solve your question please mark the appropriate reply as the Accepted Solution. 

Of course, if you have more to share on your issue, please let the Community know so other community members can continue to help you.

Thanks,
Vivek N.
Community Moderation Team.

[cgherghe-2]

This is one of the sketches I was having trouble with.
I was trying to avoid working with dimensions like 2.825568 and 0.989737 or 0.500172 -- I got around it by sketching just a quarter of it and then mirror it twice.
However, even this proved to be troublesome -- snapping to geometry is not a perfect process, not at least at my end, so whenever I had three lines intersecting they were not concurrent, but formed a little triangle, and since I had to delete some segments from the mirroring, it left a lot of opened perimeters.