question: how to 'safely' send vendors your solidworks files w/ sheetmetal?

Hi all,

I have some fairly intricate assemblies that I need to send to a vendor
who also uses sw. I don't want to send the native files because....
hmmm.. not exactly sure why. There are several folded sheet metal
parts.

Normally I would export my model as a parasolid and reimport it. But
then the ability to unfold the sheet metal will be lost unless they use
featureworks. And I'm not sure that the flats will match (never
tried).

I guess I'm really polling to see what everyone else does in these
situations.

Thanks,

Zander

 

Speaking from the vendor side, I would say to send the best you have. Think
about it from the standpoint of both of you using SW. If you did the part
as a proper sheet metal part, then all they have to do is possibly modify
the K factor for their specific tooling. Doing it this way gives you the
absolute best chance of getting the part you desire by eliminating creation
errors. If you don't trust them enough to not share your files, find
another vendor.

WT

 

Hi Wayne,

I agree and that is a good point. It is not that I don't trust them -
I'm actually removed by an entire level in this case as there is a 3rd
party between me and the vendor which will make open communication
difficult. I basically want to send it with all the dims locked (ie.
parasolid import form) but retain the unfolding / k-factor ability.

I've often tweaked k-factors for vendors until the flats match their
internal bend allowances and have no trouble doing this. I think I
also suffer from a little bit of 'this is my baby' syndrome!

Zander

 

Send them the SW file but make a copy yourself that you then lock.
When they have done their tinkering ask them to send you back 'their'
SW file. Then using SW 'compare geometry' quickly check that their
engineers have not inadvertantly 'tinkered ' that step too far away
from what you want.


TTFN

Jonathan

 

Alternatively, you can inquire of your vendor as to the particular bend
deduction/allowance for your bend radii and material thickness, and use
those values when generating your sheet metal part, generating the flat
pattern for them. I also provide several pdfs to include inspection
dimensions at various stages of the bend process.

That is what I do with our sheet metal parts, as our vendor does not
have solid modeling capability. Doing so, I've never had an issue getting
the part that I want. Most of our parts hit +-.010" in the bent condition,
which is well within our tolerance range.

 

I have had very good success with exporting the native SolidWorks sheet
metal part via Parasolids, reading it back into SolidWorks and then
appling a sheet metal feature to the "dumb" solid.

It's remarkable how well SolidWorks can often create the bends and
allow for unfolding, even with NO feature history. I've also used the
same technique with parts imported via IGES (and other formats) as long
as the translated data represents consistent wall thickness and the
proper inside/outside fillet radii to allow for flat pattern
calculation.

If the creation of a sheet metal feature fails for the Parsolids
conversion of the native SolidWorks part, you can always export (2)
Parasolids files - one in the bent state and the other to capture the
flat pattern.

In any event the objective is to avoid the inadvertent (or unapproved)
modification of a component during processing by the manufacturer...

Not providing your supplier with the native data may however require
the exacting use of agreed upon K-factor and other sheet metal
specifications during the part development within SolidWorks.

Per O.Hoel

 

All sound advice and good approaches. Historically, I've always used
sw-explorer to create a 'clean' version (with no toolbox or design
library path references), then used parasolid export and re-import to
sw prior to sending files out.

This time, I just used sw-explorer to create a clean copy. It was
less work! And the pdf of the fabrication drawing is as much a 'locked'
copy as it shows all required dimensions. etc.

Zander

 

I agree about not sending full-featured models. I have many rasons for
this. Mostly because I have been victim of customer's curious CAD
techs fiddling around and bumping things out of place. Also,
featureless models avoid the "wrong config" syndrome.

SW is quite capable of unfolding a featureless imported body, so long
as that body has uniform thickness and no odd forms. If your vendor
has enough on the ball, he will know this. f he doesn't consider it a
red flag against the vendor. There's much more to a good vendor than
CAD compatibility.

When I was designing stampings, we never sent unfolded models to
toolmakers. It was found to be counterproductive. Most toolmakers
have there own grimoire for calculation bend allowances and form
distortion. Differences between toolmakers were subtle but significant
enough. It is better to have the toolaker simply determine his own
bend allowances than to make him check your homework for bend factor
errors.

Our best simply did not use customer flat patterns. They quietly filed
customer flat patterns away and did their own from scratch using better
software and designers with more tool experience than most part/product
designers.

 

This is exactly why drawing are still a necessity. To serve as quality
control documents. This is your contract that insures you get the parts you
want. The models are an aid to the manufacturer allowing them faster
creation. You send them your models as SolidWorks and send them the
corresponding drawings as PDF.

Ken

 

Hi Per -

Seconded here. Parasolids will not often let them down. I have had
very good success with this method both as recipeint & originator.

The only "gotcha" in this method is that the engineer almost never gets
the form radius right (or the supplier needs something different -
tooling methods considered). If the "other end" has feature works,
then it's a breeze to sharpen the corners (recognize & delete) then
insert bends to control the form radius via the sheet metal definition.

Generally supplied reference data is a great help as long as "build to
print" is a reality and the criteria for acceptance.

Later,

SMA