SHEET METAL

[JASON8102]

I'm drawing a solidworks sheet metal part. It is a subpanel (4 edges bent 1.0") with about 100 holes on it. It is 32" x 24". We don't manufacture it, we buy it from a sheet metal company that makes it for us. I would like to get an opinon threaded started on what the print would look like you would send the vendor to manufacture. Forget about calling the vendor, they say they accept napkin sketches. The reason I'm asking is that there are two mechanical engineers in my company, one being myself with 20 years of experience. Do you provide a flat view, do you ordinate dimension it (fyi holes locations from the bends are not important on this part), if you said no to the flat view do you just provide a solid model and drawing, do you dimension from the bend to a hole and then hole to hole? That kind of stuff.

 

[dvd]

Provide a print of the finished part. Anything more is additional, possibly ambiguous, constraint on the fabricator. The fabricator understands how the flat pattern needs to be developed for their tooling.

 

[mechengdude]

flat patterns are a waste of time usually. The fabricator will usually recalculate everything anyway so don't waste your time showing a flat pattern.

 

[JASON8102]

Ok would you guys dimension using ordinate from a corner 0,0 or would you dimension from bend to a hole & then hole to hole?

Jason Schultz
Mechanical Engineer
Yaskawa Electric America
"It's got to be 5pm somewhere!"

 

[jistre]

Agreed. Never provide a flat pattern to a fabricator. You have sheet metal formulae that will give you things like bend radius that are used to generate the patterns, but they're worthless. What's important is what the fabricator's operator can do in their shop on their equipment on the day that they are fabricating your parts, and there's no way you can calculate that. The fabricator must constantly adjust to account for these variables.

By providing dimensions of the finished and formed part with specifications on the general method of fabrication (if you have specific fabrication details like shape of relief cuts, corners, etc. you're interested in in addition to final net shape), the fabricator's responsibility is then to provide you a part that, within tolerance, matches the prints and is the part you're expecting. If you give the fabricator a flat pattern, you're essentially instructing exactly where to bend and how to cut the pattern with no regard for their equipment and operator's quirks, and you will definitely not get the part you think you want.

Always provide your vendors with prints showing the net final shape of what you want first and let them do their jobs to provide that to you. If they need more information, trust me, they'll find you.

 

[jistre]

Your method of dimensioning should match your intention.

Let's say you have two holes. One is two inches from an edge and the second is four inches from the same point on the same edge, so the two holes are two inches apart. Your dimensional tolerance listed on the print is +- 1/16".

Now, you dimension them both from the same edge. The first hole is listed at 2" from the edge on the print, but it is fabricated in a way that puts it at 1 15/16". However, it is in tolerance, so you can't complain. Now, take the second hole that is dimensioned at 4". After fabrication, it is at 4 1/16". Again, it is in tolerance, so you can't complain. However, for the part to function properly, the two holes must be 2" +- 1/16" from each other. Because of the way you dimensioned your print, the fabricator followed instructions to the letter, but your holes are now 2 1/8" apart and you've got an entire batch of parts that won't work that you either have to throw away or pay to modify.

However, if you dimensioned one hole to the edge and then dimensioned the second hole from that first hole, then the tolerance of 1/16" would apply to that dimension and it would have to be held to the tolerances you intended.

Always dimension to indicate what's important and what you intend. If you want two holes a certain distance apart, dimension them that way, not both to a third feature. Likewise, if it's important that they each be a given distance to a third feature, dimension them that way, not to each other. When dimensioning, for every feature you need to think about what in its positioning is critical and dimension accordingly.

 

[markruble]

If you have complex bends then I would say show a flat pattern but our stuff is not complicated. Simple 90 degree bends with occasional drilled holes in the bent sides.

As for the dimensions. We use a 0,0 ordinate system. with the origin being in the lower left corner of the top view. All holes are called out using a bubble to a hole table. Some times all of our holes are the same diameter so a table is not needed. Just one call out of something like this. 0.250" diameter (25 places). Some times not all of our holes are through all holes and that is when a table comes in handy.

We use a machine shop outside of our company to have our panels machined, painted and silk screened. All we provide to them is a detailed drawing and plenty of notes. The machine shop does not have CAD so we provide them with drawings in a .pdf format. On one occasion where the panel was very complicated we sent them a solid model using eDrawings and a drawing in .pdf format. We also have one product that they so some minor assembly prior to us receiving. In the past a solid model showing how we want this assembled in an exploded view is all they need. We have never had an major troubles with them following the design.

We never dimension from the bend. The machine shop told us once even when we specify the radius of the bend it is not always exact and in our application the radius is not critical. What is critical is the overall size of the panel.

Hope this helps.

Mark

 

[dgowans]

I wouldn't include the flat pattern view because it doesn't benefit you as a company at all. How exactly would you inspect to this view? I'm dealing with legacy drawings at my company that include flat pattern views and every chance I get I'm eliminating them from our drawings.

As far as the other dimensions go, dimension the features you care about controlling. If the hole location relative to a bend doesn't matter to you, don't put it on the drawing. If you do put it on the drawing, make it reference so you won't potentially be rejecting parts based on a dimension you don't care about. You know the part's intended function - detail it appropriately.

 

[drawoh]

JASON8102,

I show flat layouts when there are corner reliefs that are not visible in any other state. Otherwise, I do not show flat layouts.

I like ordinate dimensioning on complex parts because regular dimensions can become an unreadable mess. You need to choose your dimensioning zeros and datums carefully, because bends are only located to +/-.015". Consider making one of your holes dimension zero and your secondary datum. Consider applying composite positional tolerances.

Most of our sheet metal shops ask for the SolidWorks model. They mess with the K factor and do their own flat layout. This is all the more reason to not include a flat layout.

JHG

 

[JASON8102]

Well I'll add this. What I have is a subpanel with about 100 holes on it. I didn't include a flat view and what is more important is hole to hole location, nothing from the bends. The bends are just around the sides 90deg. 1" up. I used one of the holes in the corner of the part as my 0,0. location..... all holes are located off of that. Previous versions of this done by another person at my company would dimension from the bent side all over to a set of holes and then dimension from hole to hole.......all over the place.
1.) I would think my way would be more accurate to manufacture vendor will use laser machine. No?
2.) Cleaner way to do prints using ordinate. Especially on a part with about 100 holes. No?
3.) I didn't make it as a sheet metal part in solidworks as well. Solid, Shell, and then added holes. The only way I see this as "wrong" is if we made the part in house. The vendor we use, we aren't charged engineering time....at least so they say. Half the time they only require a PDF of the drawing.
The guy that I'm having problems with was basically a sheet metal worker, hired, sent to Solidworks training and is now doing engineering work. So it's been a little bit of a battle on how something should be shown on a technical drawing. I know there are many ways but there are also just common sense ways and things we all know about from working in the industry.


Jason Schultz
Mechanical Engineer
Yaskawa Electric America
"It's got to be 5pm somewhere!"

 

[dgowans]

Jason,

My issues stem from a similar situation. Our legacy drawings were developed by a person who was creating the drawings to help him fabricate prototype parts internally. Once the concepts were proven out, those drawings got released as they were, flat pattern and all. If you have the authority, squash this behavior now or deal with the same issues again in the future.

 

[MadMango]

Origin at a hole is fine if the there are no outer constraints to worry about, but I would not make the holes your origin. As you indicate, the laser-cut hole positions to themselves will be very accurate. The slop will come from your bends, the thicker the material the more slop. In my experience working around 12ga, the tolerance can easily be +/-.030", though it can be held to as tight as +/-.015 bend to bend (more money).

Ordinate dims are great, but if the 100 holes are the same size, you can define the pattern rather easily with normal dims or a note. If the holes are all different, then a hole table makes sense, and it makes it easier for your vendor to do tool set-up as everything is in one table (sizes and coordinates).

As for the sheet metal featured model, you're using 3D CAD, you should use it as such. Your company bought you a shotgun, don't use it as a club. Inserting the sheet metal features in your model to allow folding/unfolding will help to ensure that you are creating a manufacturable part. Without bends, you'll not know of any interference from the inside bend radii if there are other nesting parts, or if a flange will interfere with another flange. You may get a part with seams and gaps in places that you did not expect. Having said all that, your part sounds like a shallow pan, probably not a huge concern, but something to consider.

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

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

 

[btrueblood]

We used Solidworks a lot at a couple of my old employers. As said by prior postings, and I fully agree, the final bent form of the part must be fully detailed, and that is the drawing that the part will be inspected to. A flat pattern is done solely for the convenience of the fabricator.

That said... At one company, we had a "captive" sheet metal shop doing our work, so it made sense to build a bend table for their equipment, and provide them with a flat pattern based on their tooling. At a later company, we would have some shops give us their bend tables, and generate flat patterns for them based on their numbers. These shops generally gave us more competitive quotes when we sent them flat patterns, and it was pretty quick for us to "push the button" and print the flat pattern sheet for them so it all worked out.

 

[KENAT]

As to the flat pattern, I'd say it's normally not a great idea for reasons listed above, detail the finished article not some process step (If you want to be able to quote a standard consider ASME Y14.5M-1994 paragraph 1.4e). If you do put in the flat label it as "NON MANDATORY (MFG DATA)" or similar (1.4f).

As to your dimension scheme this should be driven by function & made to support inspection.

I'm not a big fan of ordinates but this is one application where they can make a lot of sense.

Also a hole table might make sense.

Do you use GD&T or just +- dimension schemes?

You need to somehow locate the holes within the part so you probably will need a dimension at least the first hole to a bend (or maybe corner) but it can have a very loose tolerance if appropriate. If you don't have this then the holes can end up anywhere without you being able to reject it, this dimension can't be reference as that doesn't control anything.

If you're not using GD&T you may want to then dimension hole to hole, depending on function.

KENAT, probably the least qualified checker you'll ever meet...