Sheet Metal Design

[rburgess-2]

In an effort to standardize our sheet metal parts, I have been searching for a bulletproof model structure to accurately and consistently measure the flat state for blank sizes. Our standard practice has always been develop the part model through adding features, unbend, measure, bendback, and an unbend or flat_pattern which is suppressed. (UMBF for short) We then create a family table instance for the flat state that will be used in deliverables, (a drawing for forming operations and flat pattern geometry for export to CAM software)

 The issue with this practice is the measurement can be incorrect if features are placed after the "UMBF", the measurement feature references fail or do not regen, or are not oriented correctly to reflect the true OAL and OAW . 

The flat state includes measurements, (SMT_FLAT_PATTERN_LENGTH & SMT_FLAT_PATTERN_WIDTH), but can also be incorrect if the flat state is suppressed as the FLAT_PATTERN feature is inherently forced to the end of the model tree.

In the attached files, I added a "Bend Back" feature to keep the SMT_FLAT_PATTERN measurements "live", but the Bend Back failed when it was forced ahead of the FLAT_PATTERN. I re-arranged the features thru  PRO_PROGRAM by cutting and pasting the failed Bend Back feature to the end of the feature list. My family table instance needed for drawings and CAM is created by using the "Create Instance" command under the :Flat Pattern" drop down. I modify the resulting family table instance by removing the default FLAT_PATTERN feature from the table and adding the "Bend Back", which is toggled to a "N" value for the instance.

The relations set the inside bend radius and "material" parameter based on the SMT_THICKNESS as well as evaluate and convert the SMT_FLAT_PATTERN measurements to text strings for use in parameters.

For roughly 6-8 months, I have been using this practice for my sheet metal parts without issue. Parts created in this manner seem more robust than any other modeling techniques I have tried to date. Any Sheet metal feature can be added or removed without the FLAT_PATTERN and resulting measurements failing.

As this has been created in Creo 3.0, I do not know if this functionality has been added in later releases. Feedback of any type is welcome and encouraged. 

[Mahesh_Sharma]

@rburgess-2 

There is no much change in sheetmetal for your workflow. 

You may try adding the flatten instance to the drawing, before adding the parameters in a table, active the instance and add the parameter to the table or the note using &SMT_FLAT_PATTERN_WIDTH:FID_###. Then reset the generic model as active model.

[rburgess-2]

I may not have been clear in my original post. I am not having issues with this practice. It works fantastic for what I am doing. I am just looking for feedback on the technique in general.

[jconaway]

Providing some feedback on this technique.  I too had to use the unbend, eval, bend back on nearly every part we make.  I also have a lot of options on part shape, so flanges are suppressed based on user input.  This required multiple UMB fetaures, all wrapped with if/then statements.

When I discovered the internal parameters, I thought this is great! Finally!  Once I started documenting the parts, I noticed the flattened instance did not match the folder instance.

Your solution has simplified the process of getting developed lengths without a lot of overhead.  It is a really simple procedure.  Kind of like a reverse sheet metal flat pattern.

I appreciate PTC adding these internally.  But currently their implementation of updating these values is lacking.  Your method fixes that.

Thank you truly!!! 😁

[rburgess-2]

@jconaway 

Thanks for the response. Glad to know someone was able to both understand what I was doing and benefit from my pain. (lol) Too bad I can't get my co-workers onboard. Once saved as a startpart, (flat plate with [1] flange), life is much easier....