GD&T Question

[novaracer1]

Hi all. I'm fairly new to the mechanical design world, so please bare with me.

I have a drawing of a press-fit dowel pin. I have dimensioned the lenth and diameter with +/- tolerances. The pin has a pres-fit call-out as well.

Mt boss keeps busting my chops that "I haven't correctly dimensioned the drawing to GD&T specs". Am I missing something? Do I need to put a flattness, or, roundness, streightness, runout, profile of a surface, ect?

He won't tell me ANYTHING, I'm supposed to "figure it out on my own".

I have attached said drawing. Please help????

Thank you.
David

 

[SteveMartin]

I have to say, if you're boss is telling you as a relatively fresh engineer to 'figure it out on your own' he's a pretty rough boss. I'm all for people learning on their own rather than being hand-fed, but GD&T is not an easy concept for the uninitiated/untrained.

He's probably looking for a datum structure and some combination of position, runout, profile, etc...

You don't mention what GD&T spec he wants (and possibly don't know). You can start by asking him that, and then if there's a copy of the spec available for you to reference. Really, the only way I would expect a new designer/engineer to understand GD&T is through training, not attempting to interpret the spec on their own.

 

[pmarc]

Simply saying, you are missing relationship between features.

The fact that something is shown on a drawing coaxial for instance does not mean it will be such in reality. If you take your bottom drawing as an example, nothing really controls coaxiality of both diameters. One of them should be assigned as a datum feature A while the second one would have to be controlled by positional tolerance relative to A.

I believe this is GD&T that you are missing in this case.

P.S. Upper example would require more relationships defined since the geometry of the pin is slightly more complicated.

 

[ctopher]

IMO, a good boss will show you.

Here are some examples of what you are looking for:

http://www.engineersedge.com/dowel_pin.htm

http://www.draftingzone.com/shoppingzone/dmpgt.pdf

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[novaracer1]

Thank you all so much for the advice. I don't say what spec he wants because I don't know, as Steve stated. And if I ask him what he wants on the drawing he says "I don't know, figure it out", or "go look it up". I understand the aspecs of GD&T but applying it to a part is another thing(knowing what to use and what not). Not to mention what a particular machine shop will need, or use. These pins have been made, on more than several occasions before, from drawings with less detail than what I have on mine and ALL of them fit perfect. I think that most that have, and/or will answer this post, would agree that the advice they give comes from experience. And experience comes with asking questions.

Sorry.....Rant over.

 

[Belanger]

No need for things like straightness, circularity, etc. because those concepts are already covered by the diameter dimensions and tolerances. The only occasion for GD&T would be a position tolerance. To wit: you need to select one of the diameters (probably the smaller one) as a datum feature (label it with a datum letter) and then use a geometric tolerance of position on the 2.97 diameter, relating it back to that datum. There are optional bells and whistles you can add (such as the circled M), but I would start with that.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[KENAT]

As others mention, it's the coaxiality of the diameters that's missing as well as the location of the 'flats' relative to the diameter. You could add controls, or if it meets your functional requirements add a drawing note something like "PERFECT COAXIALITY AND LOCATION OF SYMMETRICAL FEATURES AT MMC REQUIRED FOR RELATED FEATURES" (you can tell your boss this comes from ASME Y14.5M-1994 section 2.7.3).

Not to mention what a particular machine shop will need, or use

A basic principle is to generally make the drawing so any competent machine shop can make an acceptable part to it. Now there is the odd exception in cases of IP or uncommon processes etc. but if you don't control what machine shop it gets sent to, then the drawing needs to document it such that any competent machine shop can make the part.

These pins have been made, on more than several occasions before, from drawings with less detail than what I have on mine and ALL of them fit perfect.

Just because you've had a few made to crummy drawings that are OK, is no guarantee that the next batch will be OK, especially if you have to go to a different shop. In the US & UK the general philosophy is that you dimension a drawing to essentially show what you will accept. You want the drawing to not allow any non functional parts, while at the same time not unnecessarily rejecting parts that are functionally OK but don't meet inappropriate drawing requirements. If you have a crummy drawing that doesn't give explicit requirements then you may legally be forced to buy crummy parts.

If you are in the US then he's probably expecting you to use ASME Y14.5. However, the question still stands of which edition. There are differences between edition as the standard has evolved over time, so you should ask what edition and if the company has a copy you can look at.

Try and get some training if you can. There are even some purveyors of self paced computer based training though I think it's only for the basics. There are online resources available too, you've just found one good one, here's another that has some stuff

http://www.tec-ease.com/#

and another

http://www.draftingzone.com/

However, the relevant standard is the 'bible' most trainers and authors of GD&T books and even folks on this site have their own idiosyncrasies (probably including me) so always go back to the source documentation.

Your manager seems a bit harsh, but then again so was my first boss and I ended up learning a bunch from him and I turned out fine (or some might argue not;-)).

Posting guidelines faq731-376

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

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[looslib]

I would change the chamfer angle from 45.00 to 45.
The others have mentioned the coaxiality aspect of the diameters.
The flats on the one part will need located to the center of the diameters.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[novaracer1]

The flats on the one part will need located to the center of the diameters.

Ben, how do I show this? I'm not sure I understand what you mean. Do I locate them from the center mark?

Thank you.

I have attached another part drw that shoes a datum feature and the length dims. I think the length dims shouldn't have the +/- and should be classified as "basic". Is that right? Also, am I missing anything more?

 

[KENAT]

Very crudely, something like this.

http://files.engineering.com/downlo...09-46a9-be03-b16306513d69&file=novaracer1.tif

However, it needs to be fine tuned to your functional requirements.

It may also be different depending on what standard you are working too - which you should specify on your drawing.

Also my sketch is obviously incomplete.

Posting guidelines faq731-376

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

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[novaracer1]

Thanks a bunch KENAT. I really appreciate it.

 

[KevinDeSmet]

If there are no proper inspection routines at your shop (or the shop that is making the parts) GD&T really is more drawing decoration than actual useful additions to one. If there are thorough inspection procedures though it can be a great thing.

Certified SolidWorks Professional

 

[novaracer1]

I have attached another part drw that shows a datum feature and the length dims. I think the length dims shouldn't have the +/- and should be classified as "basic". Is that right? Also, am I missing anything more?

One more question. Is there anything im missing on the attached drawing. I have made the changes I spoke of in the quote above, just would like a second opinion.

Thank you.
Dave

 

[pmarc]

Dave,

1. I do not think you really need angularity control on the chamfers. Chamfers can be simply controlled by 0.32 X 45deg. The way you did it is incorrect for two reasons:
- (M) modifier can not be applied to tolerance value inside FCF when surface element is controlled;
- angularity control is referencing datum A which is not present on the drawing at all.

2. As I stated in my first post, mutual relationship between features are still missing on the drawing. You should probably assign one cylinder as datum feature A and put two positional tolerances relative to A - one for another cylinder and second for flats.

 

[novaracer1]

I do not think you really need angularity control on the chamfers.

I told my boss that I thought that it didn't need the angularity on the chamfers, but he said they should be on there.

I do have an "A" datum on the other view; it’s just not shown on this drawing.

I was more concerned about the +/- tolerances on the "length" dimensions. Should those be a "basic" dimension or is it right the way it is?

Thanks again for the help, it is greatly appreciated

 

[pmarc]

novaracer1,

1. If - according to your boss - angularity has to stay on chamfers, than it is required by GD&T standards (ASME or ISO) that 45 degrees dimension shall be put as basic - preferably as separate angular dimension.

2. Regardless if the angularity tolerance on chamfers is needed or not, I would still leave (M) modifier out. Ask your boss, how he would interpret (M) in this case.

3. The 'length' dimensions, as are they now, are not basic and - what is more important - should not be measured in relation to any datum system. Simple two caliper measurements can satisfy the drawing requirement. If you want to tie these dims. to datum B, I would suggest making them basic and apply profile tolerance to surfaces that are at the distance 4.08 and 8 from datum feature B. The value of such profile tolerance would be 0.04 in both cases.

4. You have been still missing mutual relationship between axes of both cylinders. IMO this is the biggest defect of the drawing at the moment. One cylinder should be assigned as datum feature and second controlled relative to it by a geometrical tolerance (possibly position or runout).

5. Your last sketch do not show other views so I do not know if this is done, but also assure that there is a relationship defined (position tolerance?) between centerplane of side flats and the cylindrical datum feature axis.

Hope this helps.

 

[flash3780]

Looks like you got lots of great advice above. I just had to chuckle when I saw "CONFIDENTIAL" on top of the drawing that you posted on the internet .

It looks to me like the biggest things that you're missing are positional tolerances (as was mentioned above). There's no default coaxial requirement in the ASME standard - it must be defined. A datum and a runout would work just fine. Total runout also controls taper, so that may be of interest instead, albeit a bit more expensive to measure. I'd use a position tolerance to locate the two flats relative to the centerline datum. An MMC modifier would likely be appropriate on both the datum reference and the positional tolerance, especially if the function of the flats is venting.

I don't see a problem with the chamfer definition as it is in your initial sketch, but a basic angle with angularity wouldn't be wrong. You could actually make the angle basic without an angularity tolerance and it would be fine as long as you have a +/- tolerance on the chamfer depth.

I noticed that the root radius isn't defined at the step in diameters. It's important to define interior fillets for stress reasons, especially in parts experiencing cyclic loading. I would be sure to put an allowable radius on there.

Also, you may want to turn off the hidden lines in your flip-out view. They can be confusing.

If this pin is to be press-fit into something, you'll want to specify a surface finish of 32 microinches or better (or whatever that equates to in metric).

You may consider adding a feature to allow removal of the pin. If the pin is damaged in service, it'd be a shame to have to drill it out and make a new, oversized pin to replace it with.

 

[novaracer1]

I'm glad I decided to join the site. I am very greatful to all of you for helping me with the GD&T process for this drawing. I'm sure I will have more questions as time goes on. Thank you all again.