Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations The Obturator on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Concentricity vs. wall thickness

Status
Not open for further replies.
ME2QE

ME2QE

Mechanical
May 2, 2008
8
Hello All,

I have a small cylindrical part that has a hole drilled into it. I am trying to decide if the OD and the ID (really the diameter of the hole) should be called out as a wall thickness or a concentricity tolerance.

The part is molded out of plastic. I'm leaning towards wall thickness because the fixturing to measure it would be much easier to make.

Thanks for any help in advance!
 
Replies continue below

Recommended for you

Sort by date Sort by votes
As the designer, only YOU know what is important for the functionality of the part.

Your dimensioning and tolerance scheme should be based on functionality, not ease of making inspection fixtures.
 
Upvote 0 Downvote
For minimum wall thickness vs. hole size, true position w/ LMC works well.
 
Upvote 0 Downvote
Mint is right but just to try and help.

At least with ASME concentricity is rarely the right control except for things like long prop shafts etc. Consider if Position or one of the runouts is appropriate based on function.

Position may allow even easier gauging, especially if you can use MMC on both the hole & OD datum feature.

KENAT, probably the least qualified checker you'll ever meet...
 
Upvote 0 Downvote
Doh, Tick is right, if you're really concerned about wall thickness looking at LMC may be an idea.

KENAT, probably the least qualified checker you'll ever meet...
 
Upvote 0 Downvote
TheTick is correct that the hole could be shown with a positional tolerance at LMC rather than MMC to control the minimum wall thickness.

I would suggest that you reflect the hole in either circular or total runout using the OD as the datum. This will control the wall thickness a little bit easier than positonal.

Both will achieve the same results.

Dave D.
 
Upvote 0 Downvote
Thanks for the help guys!
 
Upvote 0 Downvote
You could use position @ LMC to control minimum wall thickness if that is your intent, otherwise total runout is a popular alternative, but my preference is surface profile ... you check the size & location of the surface all in one setup instead of 3 (Full-form check @ MMC, 2-pt check at LMC and then finding the actual center for position, or doing a runout check). You cannot, however, use concentricity ... it involves the Derived Median Line, and that's not a place you ever want to go ... it's beyond hard to check, and concentricity doesn't mean what it did in high school. In high school, concentricity means that the two surfaces remain equidistant from each other, under Y14.5, it means that you compare the location of the derived median line (not the feature axis) to the datum axis at each section along the length of the workpiece. That's a significant difference.

Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.
 
Upvote 0 Downvote
ME2QE,

Go ahead and use wall thickness if you want! If the part is not rigid then its form may vary to some degree. Using the controls for position, profile, or runout will penalize that deformed part even if it has acceptable wall thickness. As others have said "consider the function in specifying the control".

Concentricity is definately not what you want because concentricity does not control size or form... only location. For instance... the OD and ID could be perfectly straight and perfectly concentric yet have elliptical shapes where the max ID and min OD are 90 degrees "out of phase" naturally wall thickness would exhibit the extremes resulting from size for each.

If there was a wall thickness requirement one of the sizes would not be required.

Paul
 
Upvote 0 Downvote
ctopher,

Maybe I shouldn't be answering your question... forgive me but for rigid parts I would Yes! However for ME2QE's original question... with a plastic part and his leaning to specify "wall thickness" and his assertion that gaging would be easier... I would say it doesn't explain the size and "wall thickness" option.

Paul
 
Upvote 0 Downvote
Paul, the OP doesn't state if the part is (relatively) rigid or flexible. I've had molded plastic parts that weren't really what I'd call flexible.

He also talks about a hole being drilled, which would suggest reasonably stiff/rigid part, unless they just mean a hole co-axial to the OD, not specifically created by drilling.

KENAT, probably the least qualified checker you'll ever meet...
 
Upvote 0 Downvote
Kenat,

Sorry if I wasn't clear. The plastic part is molded with the hold in it. Its a pretty compliant part (soft plastic).

The hole mates to a shaft. At its smallest, the hole is already .001 larger than the OD of the shaft.

I'm not designing the part, just trying to fix the drawing so that we keep a specific wall thickness intact.

I haven't used GD&T in a while so I'm taking a long time to understand what you are all saying. Anyone know where I can get a refresher of sorts? I'd even take a class all over again if I could.
 
Upvote 0 Downvote
ME2QE, there are public seminars around N.America. Tec-Ease is a popular source (& I just happen to be a trainer there ... coincidence...). There are other instructors who contribute to this site also (see Dingy2 above for example), so they will hopefully also provide their sites for your reference. Public sessions are scattered around, so there should be something relatively near to you. Sessions usually range from 1 day (VERY quick review course) to 3 days (lots of Q&A), and a couple of providers now offer Webinars as well. Maybe I'll meet you at a seminar. Good luck.

Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.
 
Upvote 0 Downvote
Hi guys, Here is my two cents: Just dimension from the edge of the hole to the edge of the outside diameter and state the minimum edge dimension. Now inspection measures the two sizes and the minimum edge distance.
 
Upvote 0 Downvote
dingy2,

you mention to hold the OD as a datum for a runout tolerance on the ID. Is it the same if i hold the ID as the datum and runout the OD?

 
Upvote 0 Downvote
ME2QE:

The results would be the same but I caution that both total and circular runout are appropriately applied on small cylindrical parts. Your part is cylindrical so it would work.

Sometimes it is easier to have the ID as the datum (place in chuck)and perform the runout on the OD. That is from a measuring perspective.

Dave D.
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

J
  • Question
GD&T without concentricity
2
Replies
23
Views
6K
mfgenggear
mfgenggear
sendithard
  • Locked
  • Question
Miniumum wall thickness 1
2
Replies
36
Views
276
Burunduk
Burunduk
Enrico Urru
  • Locked
  • Question
Thickness GD&T 3
Replies
11
Views
317
Enrico Urru
Enrico Urru
JBecks
  • Locked
  • Question
Alternatives for Symmetry and Concentricity
Replies
16
Views
675
Burunduk
Burunduk
Jay8833
  • Locked
  • Question
Concentricity with common axis A-B?
Replies
16
Views
297
Garland23
Garland23

Part and Inventory Search

Sponsor

Back
Top Bottom