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Determine overall developed length


New member
Hi all,

I have been using the Pro/Sheetmetal module for quite sometime.
We simply could not do our work here wihtout it. Well, we could,
but not as robustly as we do now.

The problem I have been running into is calculating overall developed length of a piece in the flat state.

I can determine what each bend's developed length is, but what if I
need to give a shear size to my shear operator? Another place
where this would come in handy is to set the workpiece size of a MFG
sheetmetal file to the overall flat state size of the sheet metal part.

The only way I have been able to do this is place a reference dimension
on the flat state and reference that in my drawing or MFG file.
However, this does not work well if I need to delete or add a wall to
the part.

Is there a quick and easy way to determine the overall developed length of the entire part, rather than each bend seperately?

With all of the knowledge floating around mcadcentral.com, I am sure
someone has run into the problem as well. Any help is appreciated.



Edited by: conrat


New member
Hi Jim,

You can create an anlysis feature which measures the length between the two end surfaces.

It will update value whenever you change the shape of the part.

You all can record entire method into the mapkey so that you can achieve this by single click. and the assign this parameter into the respective 2D drawing.

Ican send you compete method created in ppt......but due to large size i can't upload it in this reply.

You can contact my by email : [email protected]


Prashant Patel.


New member

Thank you for the suggestion. Unfortunately, we do not have the
Behaviorial Analysis option. I was worried that was the only way
to do it. Looks like I might be forking over some more ca$h to PTC.

I find it a bit peculiar that PTC chooses to create a sheet metal
package (not cheap may I add) that does not do this out of the
box. It would seem to me that if you have invested into the sheet
metal package, you would expect this functionality.

Oh well, some things never change.

Thanks again,



New member
Tell me which version do ou have.

Asfas as i know PTC offer a Foundation package of wildfire 2 or 1 which includes this feature.........I am not sure about Pro/E 2001


New member
We are using 2001. I believe we purchased Pro/E years ago (like
version 10 or so...I was not here then) and are not using the
Foundation package. We have a bunch of old packages, like Part
Modeler. It is definietely an add-on option for our licensing
scheme. I get the "The option Behavioral_Modeler has not been acquired" error.

Maybe I need to see if I can upgrade the license.




New member
AFAIK an analysis feature will also fail under the circumstances conrat mentioned at first: "The only way I have been able to do this is place a reference dimension on the flat state and reference that in my drawing or MFG file. However, this does not work well if I need to delete or add a wall to the part." If flanges are added or deleted the analysis feature will either fail or give the wrong dimension.



New member
PTC needs to add the following functionality to the Sheetmetal Module:

A system created parameter for the total developed length of sheet
metal parts, that is constantly updated based on the extreme limits of
the flat state.

This would go a long way towards making sheetmetal drawings and manufacturing much better.

PTC, are you listening?!?!


New member
This has been Sheetmetals achilles heal since the beginning. There may be some way to set something up with analysis feature, and datums, but thats also a lot more work. What is so hard about from PTC's standpoint to give us 4 system parameters in every flat that contain values for theXMAX, XMIN, YMAX, and YMIN. Throw Z in if you like. Then we could figure the blank size from these if we wanted to.


New member

That would be wonderful. The max and min values would seem to be
a requirement of a sheet metal package. Has PTC ever actually had
any developers work in the sheet metal industry, or are they a just a
bunch of clowns?
(yes, I really wanted to use the clown icon)

Don't get me wrong, I love Pro/E's sheet metal module. It is much
easier to use than trying to manually calculate bend takeoffs when
placing cutouts. Prior to Pro/E, I used to calculate every cutout
in the flat. We had no 3D modeler that was used through out the
company. We only had one seat of Pro/E and that was only used by
a select group of employees who worked on custom one-off products.

Now we have incorporated Pro/E into our production environment with
every detailer (aside from two) using Pro/E to generate sheet metal
tapes quickly and accurately.

But the strength of your system is only as good as it's weakest
link. And the sheet metal module, although convenient, has proved
to be our achille's heel. When it is set up correctly, it works
like magic. But when things start to change size and shape, it
falls on it's face, requiring much more time than I really would like
to spend.

Yes, the min and max values you suggest seem like a no-brainer.
However, I have used the sheet metal module since version 20 and since
it hasn't been updated in Wildfire 2, I doubt it will be.




New member

Just one comment,you can use Datum Evaluate feature to monitor development length ... This feature doesn't require BMX lisence ... You can setup this feature as a distance between two surfaces and when you check info for this feature it shows length ... Hope it may help ...


New member

Although I still think PTC needs to add more functionality to it's
sheet metal module, your solution provides a much better way to
calculate the overall girth of a formed sheet metal part than I had
previously used.

I tried the Evaluate feature and it appears to work. You need to
place it in the flat state to get the flat size, but that beats writing
relations to calculate the size.

Another thing that I like about it is, it is a feature, which means I
can place two of these features (or more if needed) and write a program
to control which state of the part is being measured. For
instance, if I need to know the girth of a part with or without a
flange, I can create two of these features and suppress the one I do
not need.

NICE!!! Thanks and Kudos go out to kimale. My day just got much brighter...even with the rain!!!

Thanks again,



New member
I agree the Analysis feature would be the way to go. However, we
do not have the BMX extension, which is required for this to work.

When I try to use it, I get the following error:

The option Behavioral_Modeler has not been acquired.

They want way too much ca$h
for this option and management won't give approval for purchasing it.

If the evaluate feature works, it will be what we are looking
for. However, I agree the analysis feature is the best option.

We are stuck on Pro/E 2001 and Ilink 3.0 until February, when we plan
to upgrade to WF2 and Ilink 8. We need a new server before we
migrate. Hopefully at that time we can consolidate our licensing
into a new scheme where it is included.




New member
I just want to let everyone know that I think the Evaluate
feature is the way to go if you do not have the BMX option. The
only caveat appears to be that you must regenerate the model
twice. Once for the part to update, then again for the relation
to update.

Also, in case anyone wants to try it out...

If the Evaluate feature is named SIZE and the name of the measurement is GIRTH, you can write a relation like:


Also, here is a link to more helpful information on the Evaluate feature:


Creating the feature is pretty easy. In 2001:

1. Insert - Datum - Evaluate

2. Enter a name for the feature.

<div style="margin-left: 40px;">The Evaluate feature can contain multiple measurements.

3. Click Create, then name the measurement and hit enter.

4. Click on Distance - Plane, then select an edge.

5. Click Plane again, then click the other edge.

6. Click done and the feature will show up in the model tree.

You guys have been a plethora of knowledge and information, so I hope this information comes in handy.

Thanks again,



New member
The only problem with Evaluate feature is redefining a part. When you redefine the part so the surfaces used for Evaluate feature are no longer parallel or do not exist anymore, the Evaluate feature will no longer work properly.


New member

That is correct. Basically what we plan to do is create multiple
Evaluate features for each set of geometry and supress the one not
needed. This is still better than trying to calculate the flat by
adding the surfaces and adding/subtracting the bends.