How to relate parametric dimensions from one sketch to another?

[bry593]

In most 3D cad packages, this is easily accomplished by clicking the dimension from the previous sketch (as shown on the model) when editing the dimensions of the new sketch. Does anyone know how to do this in Pro/E?

 

[jvian]

You may need to explain a little more but it sounds like a simple relation. Create both sketches and then use a relation to drive one dimension of the second sketch with a dimension from the first sketch (unless this is not what your after). When in the relation window pick the previous sketch (or feature) to activate it's dimensions and then select the specific dimension you want to insert it into your relation. I find using the "switch symbols" button and manually typing the relations works best and is definitely the faster way.

Hope it helps,

-J-

 

[bry593]

Thanks J, that's what I tried to do, but I can't show the dimensions of another sketch while in sketch mode.

For example, Feature 1 is a cylinder made from sketch 1 which is a circle having a single dimension "sd0" = 100.

Feature 2 is a hole thru cylinder made from sketch 2 which is a circle having a single dimension "sd0" = 50. Note that pro/e assigned the same name "sd0" in each sketch.

At this point, i want sd0=sd0/2.

Problem is, I can't show sketch one dimensions while in sketch 2. Additionally, noting and typing the switched dimensions names into "relations" also does not work.

I suppose the problem is that when creating a new sketch, Pro/E resequences d0, d1, d2. Maybe Pro/E can only have relations internal to an individual sketch?

Keep in mind I'm running WF2.0.

 

[jvian]

Thanks for the additional information which I feel reveals your problem. I think your problem is that you are creating the relation inside the second sketch (i.e. inside sketch mode) which is different from creating the relation on the feature level. When I do this I have the same problem (actually I have all sorts of problems when using relations at the sketch level) were I cannot reference the dimensions of the first sketch. My suggestion to you is create the relation on the feature level after all features have been created. I also like that this keeps all relations consolidated and easy to find in one interface but bear in mind that the order of calculation becomes important when creating extensive relations across multiple features. I do this a lot and have found organization is clutch. Off topic but thought worth a a couple of penny's.

It can be done in sketch mode using parameters if you must but again my recommendation is to perform the relations on the part level not the sketch level.

Hope that helps,

-J-

 

[mjcole]

If you go to Tools > Relations you can select or show the dimensions and set relations as d14=d2

within the sketch you have sketcher dimensions such as sd1 sd2 sometimes kd for known (reference) dimensions. Typing the dimensions relations at part level will allow this and be much easier to do.

If you try to modify a sd# dimension from the sketch ProE will tell you that the dimension is driven by a relation. If the circle is the first thing you sketch it will have sd0 as it's id the symbol in sketch level is not modifiable as the d# model dimensions are.

Find the d#s for the dimensions you want to reference and Sketch 2 can take those as sketch relations. When the Relations dialog is open you can select dimensions from screen and have the d# symbol entered into your equations.

The d# dimension names are the real dimension values and consistently get larger whereas the sketch dimensions sd0 sd1 sd2 are created from sd0 for every sketch you make so there can be as many sd0 dimensions per feature. When you are in Model Edit mode and changing dims only the d# dimensions are shown.

Michael

 

[bry593]

Hey, that works! Many thanks J & Mike.

 

[looslib]

Each sketch has its own set of relations, so they all start at sd0.
I would create the sketches and then the features with approximate dimensions. Then write your relations using the feature dimension variables.
d0 (main diameter) = 100
d1 (shaft length) = 100
d2 (hole diameter) = d0/2
d3 (hole location) = d1/2


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[dgallup]

I try to avoid relations at the sketch level as they can require a second regeneration to propagate. It is also much easier to see & edit all the relations at the part level rather than having to go through section after section looking for them.

If you have a limited number of values that you want to reuse frequently it can be better to create them as parameters, then you can have a parameter like OAL (over all length) or OD (outside diameter) and use them in relations where ever you like.

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