Making perimeter a parameter

[empgoalie]

Need a little help. We do a lot of manufacturing of sheetmetal parts cut by lasers and plasma punches. What I want to do is have Pro/e calculate the perimeter of a sheetmetal part and make it a parameter for the part. This way, we can have the information readily available for cost estimates, etc.

 

[jeff4136]

Not something I've ever thought about but would probably copy edges and create Datum Evaluate features measuring the curve lengths, sum them in a relation, etc.

 

[jdurston]

I have heard of companies having Pro/TOOLKIT applications for this purpose. So, you may want to look into getting a developer create a tool for you or look to see if there is something you can purchase / license off the shelf.


If you happen to find any, let us know. Also, it would be useful to get the overall X, Y of the flat blank too (generate itfrom the formed version is a bonus..)

 

[gkbeer]

Need a little help. We do a lot of manufacturing of sheetmetal parts cut by lasers and plasma punches. What I want to do is have Pro/e calculate the perimeter of a sheetmetal part and make it a parameter for the part. This way, we can have the information readily available for cost estimates, etc.

in WF3

Create an analysis feature measuring a curve length, select one edge of the perimeter, then modify the selection to be the entire loop by hitting the details button and choosing the necessary settings. Save the analysis as a feature. The analysis feature will create a feature based parameter called length.

to see the result at any time, select the analysis feature in the model tree & choose RMB>parameter.

Also that "feature" parameter can be referenced on a drawing with the note &LENGTH:FID_XXXX XXXX being the fid of the analysis parameter. You can also use the name of the analysis feature in place of the XXXX. Note proe will convert the feature name back to the fid.

Edit: this only works for a single loop. If your part has internal apertures, you will need multiple analysis and need to add post regeneration model relations in order to sum the individual results.


Edited by: gkbeer

 

[wsylvester]

are you doing this in house or sending them to a job shop?





mostmachines will give a run time once they verify the cut path

 

[conrat]

If you do not have the BMX Extension, you will not be able to create analysis features. However, you can accomplish similar results using a Evaluate feature and an annotation.

What I do is:

1. Unbend the part.
2. Create an EVALUATE feature (under the Insert -> Model Datum -> Evaluate
3. Create the measurement.
3a. Name the feature DIMS
3b. Name the measurement LENGTH
3c. Do the measure using whatever measurement options you want.
3d. Finish the measurement.
4. Create an empty annotation feature.
5. Click Tools -> Relation, then change the drop down to feature and add a feature relation in the annotation such as:

LENGTH=LENGTH:FID_DIMS
(Note, make sure the LENGTH parameter exists in the part or you will end up with a feature level LENGTH parameter that is not visible to the main part)

Now, you will have a measurement that updates a part level paremeter everytime you regen the model. If you do not add the relation at the annotation's feature level, you will need to do a second regen to get the value to update if your part changes.

I know this sounds involved, but with a mapkey or doing it a few times, it becomes old hat. We do a lot of parts that constantly change size in length and unfolded girth. This has been a great way to update a part's flat size in one regen without using the BMX extension.

I do not remember who gave me the evaluate feature idea (it was on this forum), but thanks to whoever you are.

Jim

 

[empgoalie]

Thank you all for the ideas and suggestions. We are making these parts in house and we do have the BMX extension. I'll give the analysis feature a try.