Finally wrote-up my "How to Design Parts" section...

Hi Gang;

For about a year I've been working off and on on a fairly major pet web

project, an e-booklet on how to design parts for easy machining. Mostly

I put this together because of so many questions from our engineer
customers, and also because we're constantly driven crazy by bad
design, poor drawings, terrible tolerances, and on and on.


Anyway, I thought I might promote it a bit. As you can tell, many of
the illustrations were done with Solidworks, since this is our main
in-house CAD system. Any feedback, additions, comments, links to,
etc., would be appreciated. The page can be accessed through the
"Resources" section of our website or directly through the links
below:


http://www.omwcorp.com/partdesign.html


http://www.omwcorp.com/links.shtml


Best Regards,


Joe O.
OMW Corp.
www.omwcorp.com

 

A few comments are in order.

I looked at the first drawing. There is likely a big problem with it
although machinists will love it. Note that the location of the two
through holes is off the back edge of the top view. In fact the left
rear corner of the part is the origin for all the dimensions. While
this makes it easy for the guy on the Bridgeport to setup the job the
all important tolerance stackup on the part has flown out the window.
More than likely the spacing between the two through holes will be
critical to fitting a mating part. Yet there is +/- .010 on the spacing
even though three place tolerance is +/-.005.

Second, the drawing specifies a pocket. This is a manufacturing term
for a specific process. I couldn't tell you what pocket means from my
GD&T book in the same way I could a hole.

Rule No. 1. The drawing should define a part without specifying
manufacturing methods.

Finally, there is a double dimension on the part. In the top view .250
deep pocket is stated. In the front view a hidden line is dimensioned
..250. One of these should be a reference dimension.

Rule No. 2 Dimensions should be arranged to provide required
information for optimal readability. Dimensions should be shown in the
true profile views and refer to visible outlines.

This part is a good case for a section view or at least a removed
section to make the hidden bottom edge of the "pocket" visible to
dimension off of.

And of course it is common practice to place as the front view the view
with the fewest hidden lines. I looked at your web site and you are in
the USA so you would probably be using 3rd angle projection for your
customers.

 

Thank you for this document. It will be very useful to pass on to my
office. You wrote down a lot of information that was previously word
of mouth in a clear fashion.

 

Thanks for the comments. Yes, there are a few faults in the print. This
was not meant to be a "perfect" print as per CAD style guidelines (you
can write that e-booklet yourself ). The point was to show a
real-world print that would yield a decent part without confusing the
machinist and wasting time and money. Truth is, we *very rarely* even
see prints this good!

In regards to your point, I did think about the double dimension, but
liked the clarity of it. I should add a "ref." though, you are right. A
sectional view was hard to fit on this A size paper. The hole spacing
is a good point, but these are threaded holes, for goodness sake, not
precision alignment pins. There are nice sloppy screw clearance holes
that mate with them, .010 is just fine.

Thanks for the feedback though, I do really appreciate it.

Joe O.

 

Thank you for the kind words parel. I appreciate them.

Best Regards,

Joe O.

 

hey thanks for the thought and time you put into this.
you couldn't make a pdf of it? could you please )

 

On 28 May 2006 15:51:32 -0700, wrote:

Not to jump on Joe for unpaid work rather well done with good
intentions & much effort .....

There are drafting standards that probably went thru much discussion
& debate, such as the ANSI Y14 series, GM standards, ISO standards,
etc. for valid reasons before being published.
Sometimes the designers don't kow of them or the reasons. Usually
a bit of thought makes the reasons clear.

Part prints have (or should) a single "origin" datum point, usually, and
axes constraints ... all of which aid in assuring that any part made to
them will be "correct", unambiguous and clearly defined. .

"REF" dimensions for various purposes are usually fine, if so
called out, but they duplicate other information that should be
there in some clear form and do not control anything. Beware
the effects of tolerance stackups when using REF dimensions.

I checked CAD data for GM (among others) for a bit too long <g>.

Don't ask about "REDRAWN W/O CHANGE" !!!!

 

Using the number of decimal places to specify tolerances is among
the worst of practices, IMHO.
For several reasons, one being that from limited decimal places
*truncation or rounding* of the data the geometry may be wrong
if constructed from the dimensions. Another is that it can shift the
"mean" of the features so dimensioned.
It's not too bad if everything is in 1/8ths of an inch & everyone
knows that (they can guess which 1/8th is correct/nearest)
but otherwise ...
And non-symmetric tolerances too are bad except in a few
special cases.

 

Hi Neil:

I'd be happy to do that if I knew how. Is there some common (free)
software program I can use? I don't have any adobe programs on my
machine.

Joe

 

IIRC OpenOffice 2.0 may be able to do this.
Free & worth checking out. It's a bit of an update to
earlier versions ... many other file types are now supported
too.
But about getting text BACK from a PDF file ...

 

With 3D CAD the section view or removed section would be a piece of
cake and take up no more room on the sheet. Probably the clearest
representation of the part would be with an offset section in place of
the top view assuming you made the current top view the front view per
commonly accepted practice.

 

OK, Ok, I give up. I've revised the print. Have a look now and see if
you like it better ;-).

Joe

 

Joe,

I always appreciate working with a machine shop that is willing to
listen to a customer.

TOP

P.S. The guy assembling this will love you for it too.

 

Regarding your tip about using "yellow dimensions" on a white background: I
just had some experience with this nightmare. A potentetial client had over
100 C sized AutoCAD drawings (with yellow dimensions) that he printed out on
letter sized paper. They no longer existed in digital form. He wanted them
translated into SolidWorks-parts, sub-assembly, assembly, and drawings.
Needless to say, I turned it down. I could hardly even read the things with
one of those large inspection magnifying glasses.

Mike

 

Good stuff Dale. Thanks for writing. What you say is right on the mark.
This particular part (which by the way doesn't really exist, I made it
up for the example) is pretty simple, so it is not a big deal either
way. But fewer datums makes a big difference with fancier parts.

Thanks again for the note.

Joe O.

Best Regards,

Joe

 

What is it about AutoCad that makes all these yellow dimensions? Was it
a common default color? Or something in translating .dwg or .dxf files?
Amazing how often you still see them.

Thanks much for the great story and comments!

Joe O.

 

Just lazy operators who couldn't be bothered to setup plotstyle table and
map colours to black.

 

Mostly good. This from someone who was a machinist. Definitely good
reading. A sound study in "design for machinability".

Definitely agree about colors. Prints should make sense in black and
white (not even greyscale).

Definitely pay bills on time! I take care of my vendors, including the
occasional trip to purchasing to make sure the little guys get their
well-deserved and much-needed cash flow.

Contact name on print? No way. Does not belong on an engineering
print. Should be part of quote package, but not on print. My people
are not going to do an ECN every time project responsibility is
shifted.

Don't like to quote? There are more direct ways to terminate a
business relationship, but that one will work fine. However, it is in
everyone's best interest to have a well-crafted quote request. Ask for
what you want, because you'll probably get what you asked for.

 

Some features/dimensions are "functional". Dimensioning
them otherwise leads to tighter overall tolerances due to
tolerance stackup issues.
Example: a bolt pattern where something attaches. The hole to
hole dimensions may be more critical than where the where the
thing is related to some other similar bolt pattern. And the converse
might apply instead ....

BTW, Some in comp.cad.solidworks left out the alt.machines.cnc
& (perhaps) rec.crafts.metalworking crossposts so anyone really
interested probably needs to look at multiple groups. Folks in AMC
& (perhaps) RCM may have done similar or missed much of the
thread & subthreads.

 

Should be a chemical or process (or light source) to turn the yellow ink
black or something. Worth a shot <g>.