Sheet metal dimensioning standards

Anyone know where I can get some examples and standards for
dimensioning sheet metal drawings? I have some pretty complex parts
that need to be bent, and they have about 8 bends that are on different
axis. When adding dimensions off of a edge, the drawing tends to look
very jumbled up.

Any suggestions/tips appreciated. Thanks.

 

The company standards here are a bit lenient but we always show the bend
dimension as a linear dimension from the edge the operator will need to use
as a stop (as far as we can tell) they let us know if they need a different
dimension. Then we lable the bend line with the angle of bend and the
direction compared to the view UP or Down. We also add a bent profile view
and at times put a hold tollerance on the bent surfaces that need a relation
to eachother. As for cutouts on more complex parts we use ordinate
dimensioning. Sometimes there are just way too many things to dimension,
besides the fact that we use "A" size almost exclusively, so that keeps a
cleaner look. We also have the liberty to leave a few dimensions off since
we controll the plasma profiles directly, though if you are shopping it out
I wouldn't leave anything to chance.

Corey

 

I almost forgot if you have bends that aren't parallel with a surface that
they will need for the back stop we add either scribe lines or small holes
to indicate the center of the line they need to hit.

Corey

 

Here are a few standards and notes we apply to sheetmetal drawings:

Draw sheet metal parts without broken geometry. (CAM programmers hate
broken geometry)

Parts made from stainless steel or wood must show grain direction.

Dimension all formed bends, inside or outside - depending on fit with
mating pieces, and add REF to the last bend dimension.

We add an asterisk after all bend line location dimensions, in the flat
pattern, and place the following note in with the drawings general
notes:
" * PROCESS DIMENSION ONLY. NOT AN ABSOLUTE VALUE. MAY REQUIRE SLIGHT
ADJUSTMENT TO COMPENSATE FOR HARDNESS, ELONGATION, AND CHANGES IN
EQUIPMENT AND TECHNIQUE."

This note appears on sheet stock parts where the finish is to be
preserved:
"CLAMP MARKS PERMISSIBLE ON SURFACES INDICATED."

 

Thanks for the reply Corey.

Below are some screenshot examples of drawings. We use a laser to cut
our sheet metal parts from a DXF files we generate from the flat
pattern. Our standard is to dimension width and height, and any bend
lines. Holes, slots, tabs, are not dimensioned. We also label each
bend line with a number, and have a bend table above the flat pattern.
Depending on the line type of the bend, bend up would be a phantom
line, and bend down would be a dashed line. I dont like the way we do
this, and Im trying to get this changed for the future. I would prefer
to have a note that says "Bend Up" or "BU" and the angle next to the
note.

Can you post an example of the note you put on your bend lines?

The back gauge on the press brake can do up to 24". As you can see on
example 1, the standard dimensions look cluttered in the drawing. On
example 2, ordinate dimensions are alot cleaner. Next, on example 3,
standard dimensions take up alot more room then the ordinate dimensions
on example 4. The problem with example 4 is, the press brake operator
would have to pull out his calculator, and calculate bend # 8 and 7,
since the back gauge can only go 24". This also doesnt take into acct
that the press brake operator will bend the part in the same order that
the bend lines are numbered (many times this cant be done). On example
5, ordinate dimensions are used, but im not sure if this is good
practice to do this. We have had problems in the past where someone
might not realize the other dimensions are starting from the opposite
side, causing them to misread the bend line.

Is example 5 an acceptable way of dimensioning a sheetmetal part?

http://img.photobucket.com/albums/v154/3eleven/SolidWorks/bend_example1.jpg
http://img.photobucket.com/albums/v154/3eleven/SolidWorks/bend_example2.jpg
http://img.photobucket.com/albums/v154/3eleven/SolidWorks/bend_example3.jpg
http://img.photobucket.com/albums/v154/3eleven/SolidWorks/bend_example4.jpg
http://img.photobucket.com/albums/v154/3eleven/SolidWorks/bend_example5.jpg
Thanks.

 

an example
http://photobucket.com/albums/v222/cscheich/?action=view&current=421322.jpg

 

Tis funny to see inches still being used, metric man myself, as is most of
the UK now.
Last time I used inches was at school, lol, loooooong time ago, cough!
cough!

 

One thing I would add, is to have a separate folded drawing and the three
views with dimensions only on, helps to get the concept through to the shop
floor. Also mention if you are using inside or outside bends and try to
stick to one sort. Remember, they can not read your mind, luckily for me,
lol :-o Now where's that new 2005 calendar??

 

If you deal with any US company you will find that 80 to 90% use english
units of measure. We americans can't seem to let it go.

Corey

 

Pete.

We create a sheet 1 and a next sheet 2.

Sheet 1 shows the "flat state" with ordinate dimensions and number
of holes etc.

Sheet 2 shows the "bent state" with all relevant bend dimensions
and an isometric view for visualization.

If the part is small enough "flat state" and "bent state" are
created on one sheet only (sheet 1)

Eddy

 

Hi Monkey -

As you point out, there is no substitute for a good press brake
operator. If I could add my two cents, it looks like what you are
giving for them is a nice back-gage layout for the part, but I would
not undervalue a (perhaps) abridged print that shows them the finished
sizes of the formed profile.

This gives you operator a fighting chance at making a good part.
Giving them brake centerlines is great, but through that many bends,
they will need to play around a bit to get the profile right and will
also need a "final state print".

The only other ironclad rule that I personally inisit on having for a
dimensioned part is that ALL the dimensions come from the SAME _stock_
side of the part. No compromises here. When one uses inner & outer
reference points, it is very hard for parts to be made correctly as the
dimensions get distorted based on the actual stock thickness.

In any case, your people are close to you, so you can work out a system
that works for both of you. Presuming they are in house, you can
dispense with the legalese of supplying them a flat blank with bend
centerlines and pointing fingers when it does not come out right (as
often happens with a company to company method when people try to
define parts with flat blank brake layouts - avoid this at all costs).
Later,

SMA

 

What is the most common standard used for calling out bend lines? CS
print states "UP 90 degrees (symbol)" on the bend line. I dont see
where a bend radius is called out tho.

Im trying to see what most people do when calling bend lines out. I
dont like the way we do it, and it seems that alot more people want to
change our "standard".

Any more examples would be great. Thanks