casting drawing tolerance question

[duk748]

hello - our vice president has been checking our recent job (we are slow & he has nothing better to do) & he came down kinda hard on me the designer on friday after i had made a casting drawing of a part - i allowed anywhere from 3-6mm of stock to the casting before machining - i then showed my 1st datum & referenced the casting dim along w/ the amount to remove - also i referenced a 25mm dim. - he told me that i should never show what i want to remove nor should i give a ref. to the casting dims - let the foundry figure it out - also he said the 25 dim could turn out to be 22 after the casting was made - i countered that the dim could not be out that much due to the tolerance in the title block (+/-.4mm) - he told me the title block tolerance does not apply to a casting drawing - any input would be apprecaited - thank you

 

[MintJulep]

I agree with never dimension the material you want removed. A drawing has to show what IS, not what isn't.

Tolerances don't apply for the foundry? Unfortunately a lot of people seem to believe this - I've seen lot's of scrapped machined parts because the castings weren't thick enough. This not only wastes material (the foundry can melt it back down to try again with), it wastes transportation costs (your casting and your machining don't happen at the same place do they?) and machining time. Of course tolerances apply for the foundry. On the other hand, you've got to give the foundry tolerances that are realistic for the process. Assuming that you are dealing with a simple sand casting a tolerance of +/- 0.4mm just isn't a reasonable expectation.

I think that a ref to the casting dimensions on a machining drawing is ok - it lets the machine shop know where the part is supposed to be inside the raw casting.

 

[powerhound]

I agree with MintJulep, 0,4mm is totally unreasonable for a casting, probably even a lost wax investment casting. Depending on the size and type of casting this is, the actual dimension could vary 5-10mm either way. The foundry does have to work to some type of tolerance though so I would recommend a more reasonable tolerance block. This might require reconsidering your casting size though so that if the casting is at the bottom of the looser tolerance, you can still get your part out of it.

If you referenced the 25mm dimension by putting parenthesis around it, and it's not shown anywhere else on the print as a hard dimension, then your VP is correct they can pretty much make it whatever. Reference dimensions have no tolerance and they are also comprised of other dimensions stacked up and added (or subtracted...depending) together. This means their tolerances also stack up. If the 25mm dimension is the total of 7 or 8 dimensions added together then VP is also correct.

Hopefully I've understood the situation correctly.



Powerhound, GDTP T-0419
Production Manager
Inventor 2009
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[PaulJackson]

duk748,

If pleasing the vice-president is critical to your continued employment then it is certainly risky to argue him/her based on advice offered here. I would do it his way unless I had plenty of practical experience and either thought there was low risk of reprisal from my objections or I was prepared to accept the risk from those objections.

There are many ways to approach casting specifications depending upon the ultimate function of the product in terms of its structural integrity, metallurgical properties, "as cast" dimensional integrity, subsequent process registry requirements and/or appearance.

Small tolerances for profile are not uncommon for the industry that I used to work in... but in order to achieve them all of the sources for casting variation need to be addressed in terms of shrink, distortion, blow, shift, registry, balance... etc.

Before I retired recently I helped define precision hydraulic die-cast control bodies for transmissions where we specified datum features solely in the ejector side "the critical business side" of the body such that the intersection of the secondary and tertiary datum feature registries occurred in the center of the structure to minimize the effects of shrink variation across the structure. Since our objective was to achieve "the best possible" location and orientation of the valve port annulus' and the minimum required post-cast machining... we cored fastener thru holes in both the cover (~+) and ejector sides that didn't require machining (to maintain minimum wall thickness and minimize the risk of exposing porosity).

It all comes down to function... design integrity and economy. Like I said "there are many ways to approach casting specifications..." Your vice president's method may not be the best of all but it may be less risky for you to heed his advice.

Paul

 

[duk748]

hello again & thank you for all the help - i would not argue w/ him for fear of reprisal but i just wanted to be clear as to what was considered standard - the company i worked for before always made casting drawings & then finished part drawings - all our parts are made overseas & from various vendors so i was trying to make the process alittle eaiser to understand for the people making the parts - our company has thrown out all or any standards so i try to work to the standards of my previous company (force of habit) - the 25mm dim was an actual dim. not a reference - sorry for the confusion - it is becomming very hard to design/ draft any job here due to standards being either made up or changing to the flavor of the day everytime a project goes thru here -
frustrating to work under these conditions sometime when you have to consatntly get out your 8-ball & shake it for an answer - once again i thank you all for your help

 

[SeasonLee]

Regarding to the casting and machining drawing, let’s see what standard says:
Based on ASME Y14.8M-1996 Castings and Forgings, 2 Drawing Presentation

2.1 General
This Section establishes methods of preparing casting/forging drawing.

2.2 Drawings Containing Separate Views
The casting/forging requirements and the machining requirements are shown in separate views or on separate drawings. Phantom lines may be used on the casting/forging views to show the outline of the part configuration after machining (see Fig. 2-1)

2.3 Drawings Containing Combined Views
Both the casting/forging requirements and the machining requirements are shown in superimposed views. Phantom lines may be used to show the casting/forging outline (see Fig. 2-2). Notes and tolerances relative to casting/forging shall be distinguished from those relative to machining. Due to the possibility of conflicting casting/forging and machining requirements, combined view drawings should be used with caution.

2.4 End Item Drawing
An end item drawing defines either an individual part or assembly in its final or completed state. Surfaces may be cast/forged or machined to meet drawing requirements. Notes relative to machining shall be listed separately (see Fig. 2-3).

All above are quoted from the standard, sorry for I can’t post the figures publicly, I will forward the figures individually if anyone who are interested to get the figures. We are a casting/forging OEM parts supplier, a lot of parts need secondary machining by our customer, as what I know “anywhere from 3~6 mm of stock to the casting before machining” is really too much for a secondary machining.

Here is the general tolerance used on casting/forging:
X.XXX = ± .010 (or ±.015), X.XX = ±.02 up to one inch, ±.003 (or ±.005) for each additional inch.

SeasonLee

 

[KENAT]

I'm not sure I fully understood your post, but detailing the amount to remove does sound wrong, you should be detailing what remains.

One thing I'm not quite clear on, are you doing separate casting & machining drawings?

Is this where the idea of the 'tol block not applying to castings' comes in? If using separate drawings then the tolerances on the machined drawings do not apply to cast features (ASME Y14.5M1.4).

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[duk748]

hello again - the drawing i have made is one drawing & i have added dims. to show on my 1st surface to remove 3mm to start the machining - all other dims. are for machining & casting - the tolerance block on our format shows for fabrication a tolerance of +/- .015 (.4 mm) - for machined dims. +/-.005"
it is of my opinion that any nominal dim. for the casting should have no larger tolerance then +/-.4mm (.015") - any machined dims. that are not specific tolerance will follow the title block tolerance of +/-.005" - maybe i am wrong in my thinking - thank you

 

[KENAT]

What casting process are you using and what kind of size item? +-.015 sounds pretty tight.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[duk748]

i am not sure of the casting process because the part is sent out to different vendors overseas - the size of the part i cannot give you now because i do not have the drawing w/ me - i will post the dims. on tuesday - the

 

[drawoh]

duk748,

Most foundries I have investigated quote a tolerance capability of ±.005"/inch. This includes investment castings.

Any time I have done castings, I have prepared a separate drawing of the casting, and of the final machined part. I would not do otherwise unless I was confident that the casting and the machining would be done at the same site. I need to tell the foundry what I am doing to accept. I need to tell the machine shop what the raw material looks like. Casting tooling is expensive in my world, and I need to consider the possibility of an alternate machined part based on the existing casting.

JHG

 

[MintJulep]

Most foundries I have investigated quote a tolerance capability of ±.005"/inch.

It's easy to quote a nice tight process capability.

Most foundries that my vendors who use castings use seem to have a process capability of about +/- and inch or so.

 

[KENAT]

I recently was quoted +-.06, +-.09 across parting line, for an Invar casting not much bigger than a house brick.

However, I've seen very tight tolerances quoted on some small parts.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[MechNorth]

A significant problem with the old-style 0.XXX +/-0.### general tolerance blocks is that those numbers aren't usually changed regardless of what type of drawing is being done. As indicated, there are some general casting tolerances available for the industry that could be substituted in for those used on machined component drawings. It does go further than that, though. Unless you are doing very coarse castings, many foundries now have better process capabilities than those general tolerances were based upon, and so they can hold better / tighter tolerances. The benefit to this is a better casting that is closer to your final machined sizes with significantly reduced risk of sinks and other defects. Less scrap & less material removal may be available just for the cost of communicating with your foundry.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

MechNorth, I'd caution against changing standard block tolerances drawing by drawing. People get used to the default setting and errors can creep in.

I'd instead suggest putting the tolerance on the individual dimensions (or obviously if applicable use GD&T FCF's).

You might get away with adding a note giving the different tolerances for 'cast features' but believe this may be confusing.

The problem with block tolerances isn't so much that people don't change them as that people invoke them without assessing the impact/meaning.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[drawoh]

KENAT,

This is my favorite drafting rant.

Casting, welding, sheet metal, carpentry and such are not accurate processes. To prepare drawings, you need to understand what your fabricator can do, and specify tolerances accordingly. If the feasible tolerances are too loose for your design to work, your design does not work.

I agree strongly with not using the title block defaults.

JHG

 

[MechNorth]

Kenat, agree with the sentiment that errors can & will creep in. The problem that I've typically encountered is that the general tolerancing standard that was selected was so coarse (as dictated by a sister operation) that we literally would have had to tolerance every dimension individually. On a simple part, no biggie. On our parts with literally hundreds to thousands of dimensions, it was a significant effort under the +/- general tolerance system. We had to have different blocks for each operation, and within some ops there were separate casting, forging, machined and molded tolerance blocks. It wasn't such an issue for the shop and suppliers because they typically didn't see a cross-section of the different types of drawings.

Definitely prefer a general surface profile with a tolerance value established for each individual drawing based on the most common tolerance on the drawing. Minimizes the detailing time.

Overall, I find that expectations for drawing-users' abilities have dwindled to the point where we are uncomfortable expecting people to be able to read drawings. Sometimes I feel like we've dumbed down our processes (design, manufacturing, inspection) too much, and that is one of the causal factors in our current economic situation.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

MechNorth, if you saw my rant over on thread1103-238757 you'll see similar has occured to me on dumbing down.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[MechNorth]

Yup, nice rant, Kenat. I had avoided that thread initially ... must resist the temptation...

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com