How to relate parametric dimensions from one sketch to another?
How to relate parametric dimensions from one sketch to another?
(OP)
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?





RE: How to relate parametric dimensions from one sketch to another?
Hope it helps,
-J-
RE: How to relate parametric dimensions from one sketch to another?
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.
RE: How to relate parametric dimensions from one sketch to another?
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-
RE: How to relate parametric dimensions from one sketch to another?
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
RE: How to relate parametric dimensions from one sketch to another?
RE: How to relate parametric dimensions from one sketch to another?
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
RE: How to relate parametric dimensions from one sketch to another?
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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