Regarding Sheet metal drawings 1

[kaffy]

Good Morning Everybody,
I am working on sheet metal parts and relatively new in this field.I am trying to find out what the industry standards are for sheet metal drawings.
My question is what kind of drawings or documentation do you guys issue in case of sheet metal parts?
Is it just a DXF file or a DXF file and a drawing file both? If issuing both then how detailed the sheet metal part drawings are supposed to be(since flat pattern dxf file with bend lines already has most of information) ?


Thank You
KD

 

[drawoh]

kaffy,

I send out a PDF file of the drawing, completely dimensioned and toleranced, with full GD&T. I am quite happy sending a STP file of the CAD model.

Have you talked to your fabricator?

--
JHG

 

[Jboggs]

You send whatever the fabricator requires to produce the part correctly. I would suggest a dimensioned flat pattern as well as views of the finished part highlighting the critical dimensions. If your fabricator is an experienced sheet metal shop used to dealing with drawings from your company, that's one thing. However if the shop is, for example, a CNC operation that also does a little sheet metal work out back, then they might require a different approach. Put yourself in the fabricator's shoes. Give them everything they need in as simple a presentation as possible, but do not over-complicate it. That just leads to confusion and errors.

 

[SBaugh]

If you don't have a press brake at your facility I would "NEVER" send out SM files in a flat pattern. At a previous job, we did that and paid a heavy price. Because each machine is different as is the tonnage and their k-factor, etc... that may be used, caused all our parts to come out short, due to either the K factor that we were using or the dies\tonnage they used. At that moment forward any files that were being farmed out to be bent were in a native SW file or Parasolid\STEP file in the bent state. Along with drawings in the bent state. If DXF were requested in the flat state I would send those from the CAD model itself and they would have to do the calculations on it not us.

Scott Baugh, CSWP
CAD Systems Manager
Dapco, INC

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[kaffy]

Thank you guys.

 

[hendersdc]

As SBaugh says, the sheet metal house will need to put their own bend deductions into the file to work with their processes. We provide a drawing pdf, a step file, and the native solidworks or creo file. All are in the final/bent shape. The pdf and step are the controlling files in the event of unintentional modification of the native file by the supplier.

I used to work in a sheet metal shop, if the customer didn't send native files we would recreate them from scratch to be able to add the proper bend deductions.

 

[GrouchyStressedTensePoor]

We do a lot of this.

We send out fully dimensioned PDFs and DXF flat patterns. We make it clear that the drawing is the master document, and that we are providing the DXF as a courtesy. We state the K factor used to generate the flat, and it is up to the supplier to adjust the DXF as necessary (easy enough to do in 2D CAD).

We do this because we have had problems with parts that were made from "master" DXFs before, as others have alluded to above. However, in reality, if your part is sensibly toleranced, being a few hundredths off with the K factor is unlikely to make a difference for most applications.

GSTP

Graduate Mechanical Design Engineer
UK

 

[moon161]

IME, generally what the vendor/mfg needs to make a quality part or assembly. For me this has been, depending on the vendor:

-Dimensioned PDF drawing of folded part, indicating gage and material
-Dimensioned PDF drawing of folded part, details of punches, forms & louvers, gage and material
-Dimensioned PDF drawing of flat pattern, DXF for the laser.
-In the case of internal shop, Shared SWX drawings, models & flat patterns w/ mfg engineer. They would simulate the braking process to make sure it would work IRL. Typically one drawing showing finished shape, and one showing the flats with a reference dimension. The shop would burn & brake I think from .063 to .375 steel, we designed it like sheet metal with welding instead of fasteners. Assembly dwg would show finished dimensioned assy, BOM and welds.

 

[looslib]

Our drawings at a previous job for sheet metal parts would have the bent part fully dimensioned and a flat pattern with basic dimensions. The flat would be made with our internal K-factor and the drawing view was marked as being for internal use only. When we sent a part outside to be manufactured, we are buying the finished bent part, not the flat pattern. If the vendor could use the flat pattern, we would supply it to them upon request. We did work with a few suppliers who could use our flat patterns.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[drawoh]

GrouchyStressedTensePoor,

I have been asked by sheet metal shops for the SolidWorks file. I am okay with that. They then messed with K[‑]factor to make their flat layout.

I put flat layouts on drawings to show details that are hard to see on folded views. If I do not have a problem like that, I don't show the flat layout. No sheet metal shop in its right mind should trust a flat layout of mine.

--
JHG

 

[kaffy]

Thank You guys