Handling Metric and Imperial Versions of the Same Part

[axym]

Hi All,

A client has a few sheet metal parts that are each going to be made by two different suppliers. One supplier is in North America and prefers to work with Imperial stock material thicknesses and the other supplier is abroad and prefers metric stock thicknesses.

The suppliers each want DXF files of the nominal geometry. I have been told that the nominal material thickness affects things like bend radii, and thus affects certain dimensions on both the flat pattern and the final part.

The client would rather not have to create and manage two different drawings and two different DXF files for each part. Any ideas on how this type of situation is commonly dealt with?

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[drawoh]

axym,

If you are using a 3D[ ]CAD package like SolidWorks, send them the CAD files. Sheet metal fabricators find these useful. Converting from metric and English is as simple as pulling down the Units button in SolidWorks. I am sure the other packages are similar. Our vendor does this with our metric drawings.

A DXF file can be converted, by the supplier, from metric to English by scaling everything by 10/254. He will have to fix the tolerances and the fonts.

Your client should manage one set of drawings, in the original set of units, with the original tolerances.

Don't specify metal stock. Call up thicknesses and tolerances. Make sure your thicknesses overlap metric and English stock. 2mm sheet aluminium is very close to 12[ ]gauge aluminium sheet, for example.

JHG

 

[KENAT]

I was going to suggest similar, one drawing but dimensioned & toleranced in such a way to allow both the metric and inch 'stock' of required thickness to be used.

As to bend allowances, flat pattern... often best to leave it to the shop to specify this and stick with what ASME Y14.5 says in section 1.4 about detailing the finished part.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[axym]

Gentlemen,

Thank you for the input, that helps.

I investigated the issue further, and it turns out that the issue is mostly to do with who is going to do the scaling of the DXF file. I had forgotten that DXF is a "unitless" format. I agree with drawoh that any required scaling should be the vendor's responsibility.

Would you recommend using a different neutral file format such as STEP, that encodes the intended units? Is this generally better?

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[btrueblood]

"Would you recommend using a different neutral file format such as STEP, that encodes the intended units? Is this generally better?"

Yes. Though some vendors complain they can't read them.

 

[MadMango]

That depends on how advanced your vendors are. With my vendors, they like the flat DXF as a sanity check, and request IGES files to develop their own flat file... or so I'm told.

"Art without engineering is dreaming; Engineering without art is calculating."


Have you read faq731-376 to make the best use of these Forums?

 

[KENAT]

Can you do 2D step well, I forget? For 2D I usually use PDF & if they need 'CAD' I'll send a dxf as well. I never send just a DXF because some things tend to get messed up in translation.

If the drawing says what units it is in, then I don't see the big deal. Don't get me wrong, I've had a few moron facilities guys that couldn't work out why our tool footprints came through a factor of 25.4 off but well, you can't fix stupid.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[drawoh]

axym,

A DXF copy of your fabrication drawing shows intelligent dimensions, which ought to update correctly when you re-scale everything.

I am surprised your vendor does not want your 3D[ ]CAD files. SolidWorks sheet metal is intelligent. I am sure ProE/CREO and Inventor are too. Generating a flat layout requires some skill and knowledge that the fabricator ought to have. Let them do it.

I assume you can scale a STEP file, but I have never done it, and I have no interest in doing it.

At some point, if your fabricator has high end CAD software, he can model the part based on your drawing, reproduce your drawing and your units, check his drawing off of yours, and then change units. I can see no use for an unintelligent 3D[ ]CAD file, unless your part is hard to visualize.

JHG

 

[looslib]

The parts may not be interchangeable if you just do a conversion from english to metric dimensions. The material thickness will have to be adjusted to stock sizes and this could have an effect on the size of the part as well as the bend allowances. You need to look at which side of the bent part is mated in an assembly so the tolerance is designed to be on the non-mating side when converted.


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

Ben Loosli

 

[ctopher]

Create the drawing showing dual dimensioning (whatever the primary units are on top), then export flat pattern to DXF both units separate. It's OK to have two DXF files for mfg, it's the drawing that indicates which rev it is.
Send them the drawing as PDF with dimensions so they know the real size of the part. It's too easy to screw up without the info.

Chris
SolidWorks 10 SP5.0
ctopher's home
SolidWorks Legion

 

[CheckerHater]

This is not even a can, but rather 55 gallon barrel of worms, especially if by DXF you mean "flat pattern".

One flat pattern will never work with 2 materal thicknesses, unless the tolerances for final product are +- .100"/2.5mm.

And it always will be your fault, because you supplied "wrong" flat pattern.

The best you can do, is to supply drawing of final, formed part.

The drawing of the flat should be concidered "reference", with note like "Generated using arbitrary values of thikness so-and-so, bend radius so-and-so, K-factor so-and-so. It is vendors responsibility to generate flat pattern"

Sorry, but IMHO there is no good way out of your situation. :-(

 

[Walterke]

I agree with CheckerHater that giving the final dimensions of the finished part is your best bet. In the end, they are what your customer wants. Everything else is your supplier's problem.

Step file should also be useful, provided your suppliers have the required software to read/use them.

NX 7.5
Teamcenter 8

 

[dgallup]

Never supply flat pattern data. Put the requirements for the finished part in your drawing/model. If it can be made from multiple thicknesses without negatively impacting form/function then tolerance it that way. Let the supplier work out the bend allowances. Most of them (the good ones) have their own bend allowances based on their equipment and processes. If you supply the flat pattern data & it doesn't work then it's your fault even though you have no control over the process.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[MechNorth]

I agree with what seems to be the consensus position so far. Issue the final part drawing; include dual dimensions on the print, and allow variation of stock thicknesses either by tolerance or by stating the specific stock gauges permitted. The potential for a vendor getting the wrong flat-metal file is too great.
Along with STEP, Parasolid is a format commonly used by many / most CAD packages now.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com