×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Position tolerance, Double-D Hole

Position tolerance, Double-D Hole

Position tolerance, Double-D Hole

(OP)


See picture above(which hopefully posts)

I'm trying to use GD&T (Y14.5-2009) to tolerance the flats of the D-hole. What I'm trying to describe is the flats centered on the 1.125 diameter hole.

I also have to do something similar with the shaft that fits through this hole.

Position tolerance I have doesn't feel quite right. What are your thoughts?

Thanks,
Pete

(apologies to those who've seen this in a different (wrong) section of the forum.)

RE: Position tolerance, Double-D Hole

If you can live with the tolerance values to be the same (the size and the position tolerances for the entire hole), profile of a surface ("all around") is the easiest way, rather than the position symbol.

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

RE: Position tolerance, Double-D Hole

You don't really need the basic .438 dim.

RE: Position tolerance, Double-D Hole

Dimension the Ø.125 as vertical length tangent-to-tangent.

RE: Position tolerance, Double-D Hole

I would put the D on the 1.125 dia. As is it seems that you only want the one arc as defining feature for D.

RE: Position tolerance, Double-D Hole

Picking up from where I was in thread404-351660: GD&T Question...

You already have a control on parallelism of the straight edges to -B- from it being referenced in the position fcf for the .875 width.

Also as I said before .438 is not essential.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Position tolerance, Double-D Hole

I see nothing wrong with the dimensioning of flats as long as there is true functional reason to control the flats to 1.125 diameter and not to |A|B|C|. Referencing to |A|D|B| means that design intent is to have the width perpendicular to datum plane A, centered at datum axis D and parallel to datum plane B. Quite clear.

As it was mentioned, basic .438 is not needed.

Additionally diameter symbol preceding tolerance value in positional FCF for 1.125 diameter is missing.

You should also consider applying two perpendicularity tolerances controlling mutual relationship between datum features A, B and C:
1) for datum feature B - perpendicularity to |A|;
2) for datum feature C - perpendicularity to |A|B|.

RE: Position tolerance, Double-D Hole

Also consider applying flatness tolerance to datum feature A

RE: Position tolerance, Double-D Hole

I suspect B & C are really just manufacturing datums, not important to the function!
Frank

RE: Position tolerance, Double-D Hole

According to ASME Y14.5-2009 paragraph 4.9 datum features now “shall be controlled”, and according to sub-paragraph a) of said paragraph, form of primary datum feature is first on the list.

RE: Position tolerance, Double-D Hole

According to the very same paragraph 4.9 form of primary datum feature may be controlled "indirectly by dimensions such as the size of primary datum feature of size".

RE: Position tolerance, Double-D Hole

Since when flat surface is feature of size?

RE: Position tolerance, Double-D Hole

Flat surface is not feature of size, but flatness error of the flat surface is indirectly controlled by size tolerance applied to .125 dimension through Rule #1.

RE: Position tolerance, Double-D Hole

I agree that the size tolerance will indirectly control flatness of derived median surface or something of a kind.

However, using size tolerance to control flatness of ONE particular side you have chosen to be your datum feature introduces some ambiguity, don't you think?

RE: Position tolerance, Double-D Hole

No, I do not think so.
If we assume for a moment that tolerance for .125 dimension is let's say +/-.005, allowable flatness tolerance for both sides of the plate will be .010.
What is ambiguous with that?

RE: Position tolerance, Double-D Hole

CH -- flatness of a surface is indeed controlled by the size dim. It's not just the median plane, but each surface. (I can do a sketch later today if needed.)

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

RE: Position tolerance, Double-D Hole

(OP)
I'll have to make a point to follow this forum more. I think I'll learn a lot.

RE: Position tolerance, Double-D Hole

No need for the sketch.

I am just trying to say, that you have to assume the worst, unless you actually specify flatness for one side.

Now the question is "which side?" We have symmetrical part that can be flipped over.

According to another fun paragraph, 4.8, we may have to add identifying feature to tell one from another. Good thing is we "may", not "shall", but I feel slightly uncomfortable adding non-functional feature just to satisfy requirements of the drafting standard.

RE: Position tolerance, Double-D Hole

If .010 of flatness error is acceptable from functional point of view, I really see no reason of applying additional flatness tolerance - although conceptually it is quite simple tolerance to understand, in reality its verification may cause serious pain. Plus, adding it will not solve the problem of symmetrical part at all.

RE: Position tolerance, Double-D Hole

Verifying flatness of flat part causing serious pain? I am out.

RE: Position tolerance, Double-D Hole

I suspect the people who do not want to check my short pilot diameters for squareness are not going to like checking B & C for squareness to A here either.
Frank

RE: Position tolerance, Double-D Hole

You are out because of lack of pain or something else? smile

I once asked 10 different inspectors: "For a simple rectangular block, where bottom face is datum feature A and flatness FCF controls its form, how would you verify this requirement?" You know how many answered something like: "You put the part on a base plate upside down, probe the datum feature with a height gage, and report the absolute value of indicator reading"? 8 of them.

This really is a problem out there in the real world.

RE: Position tolerance, Double-D Hole

pmarc,
I think that is OK as long as it is good, right?
Frank

RE: Position tolerance, Double-D Hole

But how to know that it is good if verification method is wrong?

RE: Position tolerance, Double-D Hole

If it is good it is parallel and flat, is that not true?
Frank

RE: Position tolerance, Double-D Hole

The surface is primary datum feature, so it does not have to be parallel to anything. The opposite face may be controlled for parallelism to it, but this check is not required if not explicitly stated on a drawing.

The inspection method described unnecessarily verifies parallelism - that is first thing. Second, it is not able to extract actual flatness error from this check.

RE: Position tolerance, Double-D Hole

(OP)
To pmarc's points - this tab (bottle opener?) gets welded into a frame, rather uncritically. The hole location isn't that critical either... The Double-D itself is an anti rotation mechanism (for a fire hose fitting that I am concurrently working on) - so the hole itself is the only real critical thing here. The effort of inspecting the flatness of B and parallelism would be unnecessary unless it was so butchered that you could see it from across the street.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources