GD&T drawing feedback 4

[panzer32]

Hello, I'm a recent mechanical engineering graduate. I'm currently out of work so in the meantime I decided to study some GD&T skills (since we basically learned nothing about GD&T in school).

For practice I took a part found in my old graphics text and drew it in a trial version of autoCAD using what I know of GD&T principles. The actual tolerances that aren't specified in the original drawing I mostly just made up but hopefully are reasonable.

Here is the drawing from the text -

https://lh5.googleusercontent.com/_...AAAAAAAdk/fdPsNQcSnnU/s912/IMG_0900 small.jpg

Here is my drawing -

https://lh5.googleusercontent.com/_...o/Ork01ZT_3fM/s912/Graphics Txt Fig 11.51.jpg

I was hoping to get some feedback whether I am on the right track or not, especially with setting the B and C datums as the two holes - is this done properly? I would be grateful for whatever feedback you can give me. There are a few niggly bits which I'm not satisfied with but I'm not sure how to change in autocad, like the centrelines not having the short crosses in the centre of the circles.

 

[fcsuper]

Without looking too deeply into it, I noticed in your general notes that you list a +/- and a general profile. These two contradict each other. If all missing dimensions are to be taken directly off the model, then they should all be basic. Of course, you'll need a note saying that the model is basic. There may be other opinions about this another other points in your drawing, but they look good just from a very general and quick look.

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[KENAT]

I'd think the general profile and +- tols only contradict each other if you have the note about 'untoleranced dimensions are basic', or am I missing something?

Posting guidelines faq731-376

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

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

 

[fcsuper]

KENAT, with the general profile, my assumption was that the model is intended to be basic and that the note was just left off. Otherwise, that FCF doesn't mean anything. Or am I the one missing something?

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[panzer32]

I put that note in to deal with the 3 threaded holes that I wasn't really sure about. I suppose they can be basic too, and thus subject to the overall profile tolerance (if they need to be tighter of course I could put a tighter tolerance on them, though I don't really know what that would look like for a threaded hole).

 

[KENAT]

What GD&T standard are you working to? I realize yours is just a sketch but you should explicitly state what standard on the drawing, or for the sake of a sketch posted here mentioning it in the OP is OK.

Do you have a copy of the standard(s)?

I would suggest using position on the threaded holes. Using position on hole patterns to ensure parts matched was pretty much how GD&T started out as I understand it, so I'd stick with it. If you just attach and fcf to a thread call out you are dimensioning to the pitch diameter.

Do not dimension to hidden detail, per the current ASME stds.

In fact, I'd minimize use of hidden detail as it creates a very busy drawing - often 'less is more'.

You can't use 'basic' dimension for the diameters of holes you then put position tols on.

No you haven't indicated B & C correctly, you need to attach the same kind of anchor you'd use on a surface to the FCF.

Your flatness fcf's would probably be better coming off the surface, rather than leader to it.

It may be more appropriate to attach the datum A identifier to the flatness fcf for that surface.

You're missing some dimension, I noticed on a couple of the threaded holes but there may be others.

I'm sure that's not an exhaustive list but should keep you busy!

Posting guidelines faq731-376

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

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

 

[panzer32]

Thanks for the feedback Kenat! Unfortunately I don't have a copy of the standard or really any good resources other than about 10 pages in one drafting textbook. I don't really have the money to spend on getting a copy of the standard or using resources other than free ones I can find online. If you happen to know a good free site for GD&T resources let me know!

I am trying for the 2009 standard, though my book and some internet information is for the previous standard which leads me to some confusion.

I understand most of your critiques, thanks! One that I couldn't find was where I dimensioned to a hidden line.

 

[pmarc]

Some minor comments in addition to Kenat's remarks, based on assumption that you want to follow Y14.5-2009 std.:

- for inch dimensions leading zeros should be omitted (except for angular dimensions - but this is not the point in your case);

- for multiplied features you should use something like '4X' not '4 X';

- for other missing dimensions: I can not see basic dimension for diameter of bigger collar (similar to dimension |[ø]2.0| on smaller collar);

- if you want to keep general note for dimensional tolerances to be within [±]0.005 (which I think is not so good idea) then there is no need for putting the tolerance for four [ø]0.656 holes.

 

[KENAT]

I think you dimension to some axis of holes which are shown as hidden line.

It's a debatable one but I found your drawing somewhat 'busy' with all that hidden detail and would suggest less hidden detail and a couple extra views as needed.

I realize you may be in 2D where this takes quite a bit extra work, so you have to trade off. However, if using 3D modelling extra views are cheap so within reason take advantage of it.

Posting guidelines faq731-376

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

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

 

[flash3780]

I empathize with your lack of GD&T training in school. It's simply not taught (even though I believe that there's ample opportunity). I found myself facing the same sort of challenges after I graduated. It boggles my mind that even though I had design courses throughout college, we spent hours and hours studying QFD, house of quality, and even equipment depreciation (which I've not used much in my professional career), but we spent very little time studying how to properly communicate our detailed designs (which I use all of the time).

 

[SeasonLee]

Some further comments :

1. If all dimensions are basic on your drawing, you may simplify it by deleting the square symbolic of all basic dimensions and add a note as :
Unless otherwise specified: Untoleranced dimensions are basic
This will make your drawing looks clean and neat, not so complicated.

2. There are four places, diameter symbol Ø missed on the position tolerance callout, for all of those features the shape of the tolerance zone is a small cylinder, so the diameter symbol can’t be omitted.

3. More comments in addition to pmarc :
* Use of X to indicate “Times”---a space is used between the X and the dimension, please note that no space is allowed preceding the X.
For example : 8X Ø6
* Use of X to indicate “By”---the X shall be preceded and followed by one character space.
For example : when a slot that has a given width by a specified length ( 5 X 30) or a chamfer that has equal sides (3 X 3).

4. Dimension line and extension line can’t use the center line, this is the one others will confused as a hidden line ( dim 2.88 is one of the errors).

5. The four holes shoule be called out 4X Ø.656±.005, not depth symbol.

Thanks

SeasonLee

 

[DrCADD]

You only use Basic dimensions for positional tolerancing. Because this is a cast part, you could not basic off of the edges of it. Your idea of datum selection is solid but you would really need to know the application of the part before picking them. One of the 4 holes in the base could have been a datum as could the hole at the top of the part. You need to know how the part is to function before picking datums.

 

[KENAT]

"You only use Basic dimensions for positional tolerancing." I'm affraid that isn't correct. Basic dimensions are also used with some other GD&T controls, especially surface profile, and can be used with datum targets etc.

Posting guidelines faq731-376

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

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

 

[DrCADD]

True, but it is typically used for position and surely not used as is done in this drawing. It would be impossible to make this part.

In the first place, the part is a casting of unfinished edges. In the second place BASIC implies theoretically perfect, such as stock materials.

Making every dimension of a drawing basic is incorrect and not workable.

 

[KENAT]

The OP's drawing does have a default surface profile tolerance which arguably might mean that making virtually all dimensions basic is correct.

However, I agree in context it's probably not appropriate.

Posting guidelines faq731-376

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

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

 

[powerhound]

"Making every dimension of a drawing basic is incorrect and not workable."

This statement is just not true. If this part is cast then it certainly isn't the way to dimension it but to issue a blanket statement like this is misleading. It is entirely possible to create a part using all basic dimensions and it be completely manufacturable and GD&T legal. Holes are better dealt with using size tolerances but profile of a surface isn't illegal to use.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[DrCADD]

While I admire your service to our country as well as your title, I stand by what I have stated and you are wrong.

I hold two degrees and was taught GD&T by one of its masters who also taught it to Caterpillar Tractor.

If you are making basic dimensions off of surfaces that are truly reference dimensions (the outsides of castings) you are doing it wrong!

I teach the subject in higher education and have taught it since 1993 after taking two 400 and 500 level courses in graduate school.

Find one example to back up your claim to this drawing being done right. It is wrong.

I can find you all kinds of examples in the two books I use by Goodheart-Willcox Publishing that show the correct use of basic dimensions but that would be a violation of copyright and you can go buy them for yourself... and you should also take a class from someone who "thinks" they know it.

BASIC dimension - a dimension that is considered to be theoretically perfect.

A dimension of location used to dimension a feature of size having a tolerance.

I have worked in industry as an engineer while teaching. NEVER have I ever had an application where I did not use this for a pattern of holes to true position them.

 

[fcsuper]

"would be a violation of copyright"

Huh? Fair use covers the limited scope of the examples you could show. Or, you make briefly create a similar one yourself as an example.

"BASIC dimension - a dimension that is considered to be theoretically perfect."

Theoretically perfect, but not perfect. Right?

In practice, 3D solid models are entirely BASIC. There's really no way to use a 3D solid model effectively unless it is considered BASIC. ASME Y14.41-2003 covers this exact topic in para. 7.2

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[powerhound]

DrCADD,

You: "Find one example to back up your claim to this drawing being done right."

Me: I did not claim that this drawing was done right. Please re-read my post.

You: "NEVER have I ever had an application where I did not use this for a pattern of holes to true position them."

Me: What does this have to do with what we're talking about? You make it sound like I said you couldn't position holes with basic dimensions.

You: "If you are making basic dimensions off of surfaces that are truly reference dimensions (the outsides of castings) you are doing it wrong!"

Me: I agree with this. Again, please re-read my post. Start paying attention somewhere around the second sentence.

Try this link for some support of my ludicrous notion:

http://www.tec-ease.com/gdt-tips-view.php?q=87

Just for example, in the drawing done by panzer there is a .76 basic dimension in the lower left corner of the lower left view. The tolerance block has a default profile tolerance of .010 to A, B, and C. That means there is a .010 wide tolerance zone equally disposed about a true profile located .76 from datum A. Apply this same principle to the rest of the part. Tell me what the problem is with that.

I will remind you that I said in my original post that if this is a casting, this is not the way to do it. My issue was with your blanket statement that "Making every dimension of a drawing basic is incorrect and not workable."



Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[DrCADD]

Okay, I am not sure what the example Tec-Ease has to do with this...

Basic dimensions in the problem of this post should only be used off of the flange edges that would have presumably been ground flat to locate the patterns of holes in true position.

My point is you do not just randomly throw BASIC dimensions at everything. That is not the correct application of GD&T. Any dimension taken off of the rough edge of a casting cannot be basic. They are treated as reference dimensions as they are random and will varie from part to part.

The example you offered was a round part that was turned. That is not the same as a rectangular casting. Apples and oranges.