Allowances for Coatings : Machinist or Drafter? 2

[tommo]

I have a question, it is pretty basic - but I would like to know what the consensus of opinion is.

We make a lot of parts, through job-shops that need to be hard coat anodized, which increases the size of the part by 0.015" per surface. People having work plated will also have the same problems.

When making detail drawings for the machined part, should the drawing give finished part dimensions (after anodizing/plating) - or the sizes that the part needs to be machined to, so that after machining the required size is reached?

e.g.
Case in point: 0.750" Bore required for bushing.

1. Should the detail drawing call out a 0.753" Bore, so after anodizing the finished size is 0.750" OR

2. The detail drawing state a 0.750" Bore with a Finish notation for Hard Coat Anodizing - putting the onus on the machinist to make allowance for plating?

It's just a little detail, but makes a big difference to the final assembly!

Thanks for any hints on how to deal with this, or is there a standard convention?

 

[TheTick]

We design finish allowances into the part.

When I was a machinist, my credo was "Ask for what you want, because I will give you what you ask for, not what you want."

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[cninneman]

Where I used to work, we always detailed and toleranced the part to show the size before any coating was applied. This way the machinist did not have to take account for it.

If a finished part was needed in the assembly, due to tolerance build up, a second configuration of the part was created for that purpose.

As a side note, (you may do things differently) we always detailed reamed holes to finished size, and had the anodizer mask the holes for us. We did not want to have to account for "build up" in a hole.

 

[tommo]

The Tick!

Thanks for the quick response!

To clarify:
"We design finish allowances into the part"

You would dimension the example bore 0.753" so that the machinist does not need to make allowances?
(Just so you know - this is how I normally do my drawings)

Sorry if I appear thick, I just need to get this stuff right!

 

[Heckler]

Tommo,

I'm in the aerospace industry and it's normal to put finished dimensions and surface finishes on the print and then put a note stating dimensions and surface finish apply after anodize. Then the machine shop makes a process print to account for the coating dimensional stack. But I've noticed with some "job shops" we use that they tend overlook those small details called notes. So we end up scrapping parts....then we started doing the process print for them and that seems to work out better. So all they have to do is turn a handle or punch a button. But to answer you question: Their is a difference between a engineering print and a process print.

Best Regards,

Heckler

"Never underestimate the power of very stupid people in large groups" John Kenneth Galbraith

 

[TheTick]

Remember:
•You are the one with quick(er) access to information.
•You are the one who knows the processes the part will go through.
•You are the one that sits next to a phone and in front of a computer and with a calculator in arm's reach.
•You are the one who can best make the decision about how much allowance is needed.

Again, I say, ask for what you want.

Some drawings have hole callouts for machined size and post-finish size. Minimize the math that machinists have to do. They are quite busy enough.

 

[ctopher]

If the machined part has machined dimensions and indicates a finish of some type of plating, the dimensions will be after the plating (in your case the anodize). Unless there is a note that indicates dimensions are before anodize. We always have machine dims then usually a separate plating dwg. The is safe because the drafter does not know if the machining and plating are done at the same vendor. Or they are both on the same dwg with dash no's, in this case it is up to the planner which vendor does which process.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[Standing]

tommo,
My recommendation is to add a note that states “Dimensions apply after finishing”. Do not anodize holes. Model your parts at nominal or MMC. As a side note .015 thickness for hard anodize is really thick. Are you really calling out .015 thickness on your drawings?


Bradley

 

[macPT]

In our case, the dimensions are always machined dimensions (unless otherwise indicated in special cases).

The coating thikness is separeted information, according to relevant standards.

Although the drawing dimensions refer only to machined parts, these dimensions and tolerances take into account the coating thikness.

Regards

 

[alexit]

As someone else almost said "This is the difference between a engineering print and a process print."

For our Engineering prints, the dimensions are for a finished part - how could your inspectors do their job otherwise?

For Process prints you would indicate the machine dimensions and note an allowance for 0.015" anodize per surface is included...

 

[MadMango]

I'm with Heckler and Bradley. Use a note to indicate dims apply after finish.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[tommo]

Thanks to everyone who has replied.

Bradley:
You are correct 0.015" is VERY thick, I mean't 0.0015"

The situation started when I sent a heap of work to a jobbing shop to have a bunch of parts made. I "took the liberty" of making the drawings exactly as they should have been machined, so after plating/anodizing the parts would be the correct sizes.

I never expected the machinist to make allowances for the post machining anodizing. As much of a good machine shop as they are - they always stick to the drawings, right wrong or indifferent, except this time...London to a brick, if I didn't make allowances for the anodizing - they wouldn't have either! However, as this is a prototype - not too much damage done, as I have extra clearance - if it was 0.003 of interference I would have a much bigger problem!


We are a small company - I will discuss this with the machine shop and note the drawings as to finished or machined dimensions. I like the concept of Engineering and Process Drawings - I was not aware of that until now.

Best Wishes & Thank You!

Anyone Else?

 

[pdybeck]

Why not call out both dimensions on the print? We just recently decided to do this on some parts that are hard anodized for us. The mil spec we referred to actually recommended this. We list the "before finishing" dimension and the "after finishing dimension". We don't do this for every dimension, just the ones that are critical. If I remember correctly according to the mil spec and what our vendors quoted, holding plating thicknesses of +/- .0002" is not atypical for hard anodizing, so many dimensions can have the finished dimension tolerances built in due to the smaller thickness of the finish (.002), tight tolerance of the finish, and loose tolerance of the machined dimension. In our notes, we call out the plating thickness and tolerance. This method works ok for us on processes like hard anodizing, but I'm not so sure on platings with geater tolerances than the machined dimensions. By calling out both dimensions on critical features, our machine shop is happy, the vendor is happy, and inspection is happy as they have something to check before it goes out for finishing, and when it comes back in.

 

[EngJW]

Like Pdybeck says, a couple of companies I worked for dimensioned before and after coating. For example, right at the feature:

Machine to .xxx/.xxx
.xxx/.xxx after coating

In some cases, say a .750 shaft running in a bushing with .001-.003 clearance, if the coating is only a couple of tenths thick, you could disregard the effects of the coating and just call it a .750 shaft.

 

[pdybeck]

jlwoodward,

A perfect example of what I was trying to explain. Thanks.

 

[ctopher]

If the anodize spec is called out with type and class, I believe the anodize thickness isn't called out on the dwg... it would be redundant. I would have a machined part dwg, and a separate anodize dwg, there would never be any confusion with the machinist or inspection.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[Standing]

Chris,
If you look at the MIL-A-8625 spec you will find that it says “As specified on drawing”, for thickness.


Bradley

 

[ctopher]

Bradley, can you direct me to where it says that? I just read thru it. I can not find it.
thanks

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[Heckler]

IMO, putting the process dimensions and engineered dimension on a single print could create more problems than it solves. I see them as two discret processes not something that should be combined. Along that same line, I've seen both casting drawings and machined drawing combined and it's sloppy at best. It goes alone with telling a machinist what size tap drill to use.

Best Regards,

Heckler

"Never underestimate the power of very stupid people in large groups" John Kenneth Galbraith

 

[pdybeck]

Heckler,

If we wanted to be purists about drawings, then I agree that you would want to split the single drawing into 2 drawings. Some might argue that they should even be separate part numbers, such as your casting and machining example. We actually do that here - casting one part number and one drawing, machining another part number and another drawing. I would imagine that is pretty common and it would definitely be crazy IMO to combine them on one drawing. For the example(s) I gave above - it is more practical to have the dimensions on one drawing if it is just a few or even one critical dimension. I say practical, because when you look at the large amount of drawings that this could pertain to in a company like ours, it would be much more time efficient to not have to create and manage tons of other drawings just for a few or even one dimension on each. There is an inherant cost associated with drawings - paper, ink, time to create, time to check, time reserve part numbers, time to enter MRP information, time to file hard copies, etc...That is the reason why tabulated drawings are often used for certain circumstances. I guess for us its just not something that is a clean cut, hard and fast rule as to when we do this, but rather a combination of a lot of factors. I'm sure every company has different thoughts on this and thats why we see in this discussion a good spectrum of differing views.