Compensating for hard anodize or other plating on parts

Hello All, I am fairly new to designing with Solidworks. I wanted to
ask, what is the popular method for compensating for anodize or other
plating on a part. For now, I have been changing the dimension so
when the part is hard anodized it will be the correct fit. But this
means that my models are 'manufacturing' level, not finished part. I
thought of creating a derived configuration for the anodize, but
haven't tried it yet. Is there a possibility that Solidworks could
implement this as a function or is there a third party app to shrink
the part, including threads? What do you think?

Thanks in advance,
JR

 

Here is the rule I go by:

If a part with a particular part number can be placed in a box with
other parts with the same part number then both parts can have the
same part number.

What you probably have is a part with a particular part number where
the print for the part is used for both machining and for the finished
part. If you can't place the machined part in the same box with the
parts that have the anodized coating then the two should not have the
same part number. If the two can't have the same part number then the
machined part should be one configuration and the machined and
anodized part should have the same part number.

Example:

Machined part -- 1000001
Anodized part -- 1000002

Then you have different dimensions and perhaps tolerances applied to
each configurations where applicable. If you use CNC then you might
have this:

Example with sub config:

Machined part -- 1000001
CNC Geometry -- 1000001-CNC where all dimensions set to middle
of tolerance.
Anodized part -- 1000002

 

I think your reply partly depends on whether you manufacture the parts
in-house.
If you send a drawing of the finished, anodized part to a machining supplier
and you leave them to deal with the anodizing company, then you will only
ever see finished parts.

Separate part numbers would (or might) only be required if you wished to
place separate orders for the machining and anodizing operations. I said
"might", because even then you might get the machining company to deliver
the parts direct to the anodizers, so there would never be an issue of
having finished and unfinished parts in your factory.

Getting back to the original question, in general I would model parts at
nominal size.
e.g. a 10mm hole with an H8 tolerance would be modelled as 10.000mm. Only
the dimensional tolerance would show the range.

If you want to use the model geometry to directly drive the programming of
CNC machines, then you probably need to model it at mid-tolerance. This
also might be useful if you need to accurately know the overall length of a
precision assembly e.g. to know if there is adequate end float.

Aside from these requirements, for precision plated parts, I model at the
nominal plated size and then add a second dimension which shows the
pre-plated tolerance.
For the parts I design, there are usually only one or two dimensions where
the plating thickness is significant compared with the finished tolerance
e.g. for bearing fits.

John H

 

I tend to agree with John H. Unless you're trying to drive the CNC
programming in-house, I would let the machine shop deal with the
finish. Specifically, I do this with a combination of notes. First,
in the title block I have a note specifying that all dimensions apply
after plating. This mean means that no matter what the variation in
plating thickness the fabricator is responsible in holing tolerances
on the finished part. Second, if pin or bearing fits are required I
use a number note specifying that this hole/feature is to be masked
prior to plating. That makes it a little easier for the shop to meet
tolerances since they don't have to worry about the additional
tolerance added by the plating.

 

If the supplier is drop shipping to anodize for you IMO it only causes
more problems than it solves.

You get finger pointing between machine shop and plating shop when
things go wrong and with hard anodize that can be a real issue.

Tom

 

John,

Reading closely what robinson said I think he is machining and then
plating or having it plated. To keep things separate in house you need
two part numbers.

 

Thanks for everyone's advice. The machine shop uses my solid model
for programming the geometry of the part. I specify the thickness of
anodize on the drawing, and handle getting the parts anodized from
time to time as well. I would like to create the part in finished
size, but provide the shop with a solid model with compensations for
anodize so they don't have to compensate.

So basically it seems that I have to model the part as a finished
part, then create a derived configuration and modify the dimensions of
the derived config. I'd give each a separate part number, and each
drawing would be labeled as 'manufacturing' drawing and 'finished
part' drawing.

It sure would be nice to be able to shrink a part if it could be done
properly.

Thanks,
JR

 

JR,

On the SW support site there is a macro available that will set your
geometry at the middle of your tolerances. This is imperative for
machining. As you mentioned you can put this geometry in a derived
config and then have another config for the anodized part. My practice
is to put specially dimensioned version of a part in derived configs
and to put functionally different versions in top level configs.

 

You can do this using "offset surface" and selecting all the surfaces. I've
tried it on a simple and a slightly more complex part (100 surfaces) and it
works fine.
To easily select all the surfaces, change the display to wireframe and drag
a select box around the whole part.

I was also pleasantly surprised that it did the "100 surface" part
instantly, so maybe there isn't too much of a performance hit.

John H

 

Offset works nice if you model faces are all offset in the same
direction. This is not always true. And if some features are modeled
at nominal and some at one extreme or the other this becomes a bit
tricky to do. Using SW to set to nominal based on the intent built
into the model automates having to do this manually and is harder to
miss something.

TOP

 

Shrinkage would be a linear function while your
coating is a (presumed) constant thickness.

Bad idea IMO.

 

Can you give me an example where this would not be the case when plating a
part - I can't visualize one at the moment....but I haven't tried too hard
either!

John H

 

Not when plating a part. Just when maching the part in the first place
to print.

TOP

 

Robinson,

This is much easier than you think. ASME Y14.5M-1994 simply states:
"Where a part is to be plated or coated, the drawing shall specify
whether the dimensions are before or after plating." For example,
have a general note that says "DIMENSIONAL LIMITS APPLY AFTER
FINISHING."

But it's even easier than that because you are right about the drawing
being for a finished part and not a manufacturing stage of that part.
A drawing should neither describe manufacturing processes. It should
only state the final condition (specs) that the part must meet. So,
if finishing is called out, it can be safely expected that the vendor
understands your spec's on the drawing to apply to the finished part.
If you are unsure as to whether your particular vendor will understand
this, talk to them before placing the order. I've been doing this for
almost two decades, and I've never had a vendor misinterpret a drawing
in this way.

Matt
http://sw.fcsuper.com