×
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

Profile tolerance vs linear tolerance - (GD&T newbie)

Profile tolerance vs linear tolerance - (GD&T newbie)

Profile tolerance vs linear tolerance - (GD&T newbie)

(OP)
I'm obviously very new to GD&T and have questions regarding linear tolerancing vs profile tolerance. I have a customer who has a print that has different linear tolerances (depending on length. The part is a casting). Based on length, the linear tolerance is as follows:


Length Tolerance
0-25mm ±0.25mm
25-50mm ±0.33mm
50-76mm ±0.41mm
76-152mm ±0.64mm
over 152mm ±0.76mm

The print is calling out a profile tolerance of -0.3mm/+0.7mm. The part has overall dimensions in the 76-152 mm range. Is there any conflict between the two? I am assuming there is as my linear tolerance allows me to be ±0.64 mm but am not sure how the profile tolerance comes into play. Thanks in advance for your help!

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Odiemena,

I would assume that the more accurate tolerance controls the feature. In other words, your part should conform to each and every tolerance called up on your drawing.

JHG

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Odiemena,
The answer depends on what the print is really showing = how profile tolerance is actually applied. Is there any chance we could see the drawing?

RE: Profile tolerance vs linear tolerance - (GD&T newbie)


Odiemena,

I assume your tabulated tolerances are placed somewhere on or near title block and represent “general tolerances” or “tolerances, unless otherwise specified”.
Normally they only apply to dimensions without direct tolerances or geometric requirements.
Any other tolerance values or GD&T symbolic will override your “title block tolerances” for feature they are applied to.

Like pmarc mentioned, it is better to look at the drawing to be absolutely sure.

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

CH,
If profile tolerance is applied to top surface of block's height and that height is controlled by simple size dimension then both tolerances may be valid since total amount of profile tolerance (1.0) is a refinement of size tolerance (1.28). That is why I wanted to see a picture.

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Quote (pmarc)

If profile tolerance is applied to top surface of block's height and that height is controlled by simple size dimension then both tolerances may be valid

If I understood correctly, the print specifies unequally disposed tolerance zone, which, according to the standard, is applied to basic profile.
I doubt you can create basic profile using “simple size” dimension.
I hope now we both agree that it may be beneficial to look at actual drawing.

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Correct, CH.
I goofed this time.

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

(OP)
Thanks for all the help guys! Here is the print for the part in question:

http://www.flickr.com/photos/29668265@N02/7349382502/in/photostream


RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Odiemena

Note 16 means Bilateral Unequal Distribution on the profile tolerance.

The profile general callout is |Porfile|1|X|Y|Z| and the tolerance 1 is divided into 0.3 and 0.7, where 0.7 is always on the added material side.

Take shaft Ø15 (external feature) as an example, the max dia=Ø16.4(0.7x2 plus 15), the min dia=Ø14.4. For an external feature , the added material is on the outward of the true profile.

Take hole Ø15 (internal feature) as an example, the max dia=Ø15.6(0.3x2 plus 15), the min dia=Ø13.6.
For an internal feature, the added material is on the inward of the true profile.

Hope this help

SeasonLee

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

On the print, as it is now, note #15 adds no value. There is not a single directly toleranced dimension to which these tolerances might refer.

Two additional comments:
1. In my opinion note #16 should contain a statement like "UNLESS OTHERWISE SPECIFIED..." at its very beginning since there is another profile tolerance on the print - |prof|0.51|Z|A| - and it is not clear whether both profile tolerances, as stated in #16 and 0.51 one, apply to the surface described by basic R127 dimension or just 0.51.

2. On section view C-C positional tolerance at LMC is applied to a feature described by basic dimension. This is illegal callout. Either 16.51 dimension shall be directly toleranced (and then the general tolerance +/-0.25 from note #15 could apply) or positional tolerance shall be switched to appropriate profile of surface control.

RE: Profile tolerance vs linear tolerance - (GD&T newbie)

Odiemena, you are in good hands smile

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