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

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

Zander,

You have two options.

You can send parasolid versions of the parts and the shop should be able to import the files and create sheet metal parts from the imported files. This can be done by importing the parasolid and then using Insert Bends to make the imported geometry a sheet metal part.

Alternatively, you can send the native SolidWorks files. I personally send native files to machine shops on a regular basis and its appreciated because the shop can create flat patterns and directly modify the bend characteristics without having to go through the steps described in the first approach.

If you're concerned that the machine shop is going to modify the designs while manipulating the native files, you should note that they are just as capable of modifying the designs when working with imported geometry. When working with imported geometry, there may be a slightly higher probability of design changes due to the occasional inconsistencies caused by file conversions.

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.

Who's paying your salary to create the sheetmetal part? If it's you or your company, have all parties sign a none disclosure agreement. If another party is paying you, it's theirs to do what ever they want.

Keith

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,

I agree completely. I do as you suggest all the time and any discrepancies are the responsibility of the sheet metal shop.

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