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Part size relation or parameter


Part size relation or parameter

Is there a way to extract the overall size of a part in x y & z direction automatically and make it a parameter or a relation?

Not directly, it can be done using modelcheck or JLink customization. In my company we use a relation to bind the outer dimensions of a part to a string parameter. Example: dimension = itos(d1) + "x" + itos(d2) + "x" + itos(d3)

Here is what I do: type this into the relations: (do, d1, d2 are the dimension of the first feature that defines the overall size) length=d0 width=d1 height=d2 Then verify the relations, PRO E will add them to the parameters as user defined parameters. I will use this information for my bill of materials. You can also use these parameters in notes on a drawing. Example: create a general and type in, &length X &width X height

Another option is to use the Analysis > Measure > Distance. In the lower left hand corner of the Distance dialog box you can select Quick, Saved, Feature. Feature will actually create a feature in the model tree of the dimension taken. WF3 M140

itos function will round off the dimension to the nearest integer. Is there any way to convert the exact value into string?




unfortunatelly rtos function is missing .

Martin Hanak

Martin Hanák

Hi Roland,

First of all sorry for late reply,

You can get the Model SIZE with a Parameter called "OVERALL_SIZE", If you want it update immidiately after every regeneration you can configure ModelCHECK to update the Size.

Model Size.jpg

Then you can make an Annotation in your Part Template as Model Overall Size = &OVERALL_SIZE

But ProENGINEER is not having intelligence to indentify what kind of Geometry it is like Circular or Non-Circular.

If Non-Circular we need to specify the Size as LxBxH

If Circular Ø DxH

By default ProENGINEER can't do this differentiation, You need to write a Relation for this.

Otherwise there is a Software called SMARTAnalysis from B&W Software GmbH, Which can differentiate the Shape of the model as Circular & Non-Circular.

It will automatically gives the size as Ø DxH for Circular and LxBxH for Non-Circular.

If you want I can send the ModelCHECK settings I use.

If still you want to know more you can mail me @ - or

Could you send me a demo video for Model check in creo 2.0.

I have a problem,to applying multi color in part using the offset features to control via parameter, it took more time. Do you have a any idea for this......

Actually, ProE does know it, but I don't know a reasonable way to get to it. As I suspect you know, the info Model Size is the length of the diagonal of the part's bounding box. The bounding box can be found in the file header. Look for:

@bounding_box 33 2

2 33 [2][3]



You can see this is the coordinates in hexidecimal of the two corners of the bounding box.

But, don't know how you could use that to get what you want.

In-fact ProENGINEER can get that intelligence, If we make some Configurations [Parameters & Relations] in the Part Template and we've to use that template as the default template for creating any Parts.

Otherwise getting the Automatic Part SIZE calculation is a bit harder.

So SMARTAnalysis will do that for us.............

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