Dimensioning stock extrusions

[nrostrander]

First of all, let me just say that after using many sites to find answers to engineering questions, I would like to give everyone on this site a big "thank-you" for being the most knowledgeable! Now on to my question.

I have been working in the aerospace industry for over seven hard years. The company I work for now, had no standards in place when I came on board. So I have been very hard at work trying to train people as to ASME and ISO standards. Everything has been going good until this new contract. One the the new people was designing a mount using stock extrusion. When he documented the extrusion, he told me that you don't dimension the extrusion parts that are not "toutched". I told him that just because you use it as stock, does not tell the manufacturer not to touch the areas. He them told me that he will just list the overalls as referance dims. Has any of you ever seen this done like this? I was tought to alwasy fully dimension the part. To me, I could then turn around and say to order stock sheet metal of a certain LxWxD and just dim the holes added?

So heres the questions:
1. Have you seen this done before?
2. Where in the standards would I find info about using stock extrusion to just put holes in?
3. Would I be correct into stating that "stock extrusion" is nuthing more than just that, a starting point? Because, if the stock extrusion is not readily available, without dims, one could not manufactur the part.

P.S. Example attached.

V/R

Nate

 

[ctopher]

Stock material features should be reference, as needed.

Chris
SolidWorks 08, CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[SeasonLee]

1.The extruded L-shape raw part will be considered as a stock per ASME Y14.5M standard 1994 paragraph2.7.1.3, so the Rule #1 does not apply to the stock.I think you should specify all necessary dimensions on your machining in house.

2.Basic dimensions missed on the positional tolerance callout.

SeasonLee

 

[nrostrander]

SeasonLee,

Your absolutly right about the lack of basic dims. He also did not properly align datum "A" eaither (flotting off the part).

So as I understand it, the stock should be dim'ed as referance.

I attachted an updated drawing with ref's and basic dims. Let me know if this is more copasetic to you all. I am going to use your replies to help teach him. As for his GD&T skills, they are inexistant, but thats just due to lack of training.

V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[SeasonLee]

1. The positional tolerance callout should be placed below the hole size dimension. You are in line with the hole size dimension.

2. 2X should be in front of the dimension .41. Please go to paragraph 1.9.5 of the standard ASME Y14.5M for more detailed information.

3. Please don't forget dim 1.00 (from datum B)is a basic dimension as well.

SeasonLee

 

[SeasonLee]

I almost forget one more important thing on tolerance expression:

The basic dimension value should be expressed with the same number of decimal place as the tolerance, please ref to the standard on paragraph 2.3.2 (d) page 25. On your case, the positional tolerance .005 has three decimal places, so all of your basic dimensions should be changed to three decimal places accordingly.

SeasonLee

 

[nrostrander]

SeasonLee,

Thank you for all your help. I was never fully tought GD&T myself, sort of self-tought. I have been learning a lot, and have no problem designing using it, but teaching others GD&T is not my strong side. I think I will have him take a GD&T course, and perhaps get myself into it for better clarification. The down side to the company I am working for, is that most people have the lack of pride in their work. Also, your right about the three place decimal. I cought that myself this afternoon, and was wondering as to how I missed it prior to then. I suppose it was after seeing it wrong so many times on all the drawings I am reviewing, it was wearing me out to the point that I was missing alot.

Drawings for review: 1541
Reviewed so far: 89
DWG's remaining: 1452
(progress takes time)

V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[powerhound]

nro,

You may want to re-consider using that point as a secondary datum. I would either switch datums B and C or change the FCF to callout the position WRT A, C, and B.

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

 

[cadman1964]

Correct me if I'm wrong here please but, the 1.00 dim on the right side should be removed and a overall dimension should be added. Reason: You have the 1.00 dim (Should be Basic) from datum "B" to the hole then 7.53 from that hole to the other. If you add a overall dimension the 1.00 on right side isn't needed. Plus who ever ordering the material doesn't have to do math to order material.

And for the reference dimensions for stocked, or purchased items. We here do use that method as shown in your second attachment. Only thing i meant do different is call the stock size out in the BOM and just dim the two legs as reference.

Solid Edge V20

 

[ewh]

I agree with cadman1964. Remove the RH 1.00 dimension and giva an overall length.
I would only reference the lengths of the legs, and that would only be to define the part envelope. If this had to be made from scratch, the standard from which it was chosen would be used for any dimensioning. To show all dimensions is an unnecessary cluttering of the drawing.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[SeasonLee]

cadman1964

Yes, I think you are right

SeasonLee

 

[MechEng2005]

Where I am, we don't follow any standard or have access to them, so please be gentle if I'm asking questions which have been spelled out clearly in the standards. We also don't typically use GD&T, so what knowledge I have is self-taught (Thanks to the regular posters here too!)

I agree with Cadman1964, although I'm not sure that having the 3 dim.s is incorrect. It just seems to make more sense to have it as he specified. Personnally, I'd leave the 1.00 dim on the right as a reference dimension (as long as it's not cluttering the drawing) and add the overall dimension.

Also, would the 1.00 dim from datum B need to be basic? To me, it would seem that the hole spacing is the critical aspect, and the excess on either end doesn't need to be held to the positional tolerance shown. I'm guessing without knowing the function of course. For example, if the title block tolerance were +/- 1/32... I'm guessing that if the LH was 31/32, there was 7.53 between the holes, and the RH was 1 1/32, the part would still function. By making the RH 1.00 dim basic, you are increasing the accuracy required without any benefit.

Is it required that all dimesions from a datum to a feature with positional callout be basic? If so, could the centerline of the LH hole be used as datum B to allow the 1.00 dimension to have the looser tolerance?

--MechEng2005

 

[cadman1964]

I agree with Cadman1964, although I'm not sure that having the 3 dim.s is incorrect. It just seems to make more sense to have it as he specified. Personnally, I'd leave the 1.00 dim on the right as a reference dimension (as long as it's not cluttering the drawing) and add the overall dimension.

Having 3 dim's is not incorrect but the 1.00 on the right has to be reference. OAL would be nice for ordering.

I've attached a image from the ANSI standard (Page 85), hopefully this will help a little. Basically you GD&T feature tolerance is your hole position tolerance up and down and all round, understand??

Solid Edge V20

 

[cadman1964]

opps forgot 2 things
1 Your dimension from Datum B does need to be basic
2 the file.....

Solid Edge V20

 

[nrostrander]

Well everyone, here is the current update. We decided to go with fully defining the angle, so that other stocks of the same material will be usable if the standard stock is not available at the time.


Feel free to comment. %-)

V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[ctopher]

If the stock dim's are not indicated as reference, they are subject to inspection. You may not always get the same stock every time.

Chris
SolidWorks 08, CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[nrostrander]

"If the stock dim's are not indicated as reference, they are subject to inspection. You may not always get the same stock every time."


Chris,

That statment is very true. Thus for our reasoning as to fully "constraining" the final part. I for one would rather fully check a part that was made from stock and find errors rather then just say "it was a stock dim, so ref it". I personnaly have found cases that the stock material was not within tolerance of our required finnished part, but they never knew that till it was too late. I beleive that one incedant cost the company over ten thousand dollers to have every part re-manufactured to be within spec. Talk about a bad delay.

V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[KENAT]

nrostrander, a work around for the issue Chris points out is to have the extrusion as 'alternate material' and a note about dims being 'stock' if it's used. Just spec the material grade and if necessary spec as the default material.

Also I think you want 2X.063, or you're missing a dim.

Mecheng - the matching decimal places is in ASME Y14.5. Also yes, the 1.00 from B needs to be basic. Essentially all dimensions locating features toleranced bye Position have to tie back to the datum with basic dims. (can be stacked basic dims as basic dims have no tolerance)

As to the idea of changing the dimension scheme and/or datum there are several options such as making the holes the secondary & tertiary datum or making the pattern a datum but this would have to be decided based on function and there's no point using a more complex dimension scheme if no one understands it, even if it is more 'correct'. If what they have adequately meets function and is adequatly understood it may be OK.

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[nrostrander]

Kenat,

1. As for the 2X .063, your right. That will need to be defined.
2. As for using the hole pattern as the datum, I look at that myself, until the designer stated that the distance between Datum C was important for fit, more so then the other end. Also, ther is another part that gets made out of this one as a "mod" that needs the Datum C. So we are leving it to allow one part to be used to make the other. I personnaly don't care for there method there, but just getting people to used GD&T is hard enought. Thus we are trying to keep it more basic untill they get the hang of it. I would rather have satisfied customers and gradual training, rather then the other way around.

V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[SeasonLee]

Nathan

I am not quite sure is it allowable with basic dimensions on the rectangular coordinate dimensioning, some dimensions (.41 and 1.00) without dimension line while the other (7.53)with dimension line, it looks very strange for me, expect someone who can give the right guide.

SeasonLee