×
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

Bend Radius Tolerance
2

Bend Radius Tolerance

Bend Radius Tolerance

(OP)
Given the shown information, what would the lowest acceptable value be for the bend radius?

Travis K.

RE: Bend Radius Tolerance

So you are asking what the minimum radius is for the 'R6' bend?

Tricky.  The 'R6' is not indicated as basic from what I can see - so it's debatable if the 'unless other wise specified' surface profile really can be used on it.

However, if you assume the 'unless otherwise specified' note is also meant to imply that all dimensions are basic, then you'd apply the 4 surface profile and your minimum radius would be 4, but this is making a big assumption.

This drawing has a lot of issues and appears to be prepared by someone that doesn't have a good understanding of GD&T or general drawing principles.

The way the 'B' and 'C' are labeled and then used looks questionable.

Also - all the [0 1], [0 2] & [0 3] are confusing to me, why are they not just 0?

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: Bend Radius Tolerance

(OP)
Kenat,

Sorry, the title block had to be cut off for confidentiality reasons. All dims are basic unless otherwise specified. Assuming that the profile tolerance does apply to the bend radius, would it be treated as a ± dimension making the radius 6±2, or would it be treated as a standard profile tolerance making it a bilateral zone equally offset in both directions from the theoretical perfect?

Travis K.  

RE: Bend Radius Tolerance

It would be treated as a standard profile tolerance making it a bilateral zone equally offset in both directions from the theoretical perfect.

However, simplistically in this case that's equivalent to 6+-2 unless I'm over looking something.

It's not a controlled radius so the surface could bobble back and forth a bit.

Though, that said, I based my comments on my understanding of ASME Y14.5M-1994 - if you're using a different standard that might make a difference because of rule 1.

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: Bend Radius Tolerance

(OP)
Kenat,

We are using ASME Y14.5M-1994. I have attached another drawing showing my concern. We used a 3mm punch to form the parts, which does not fall within 6±2, but as shown in my drawing it falls within the 4mm zone established by the profile. Do I have the wrong understanding of how profile tolerances work, or would this be acceptable because the radius falls within the established zone?

Travis K.

RE: Bend Radius Tolerance

twkinfected,

   A profile tolerance is sort of like a ± tolerance, but not quite.  

   I modeled your corner in SolidWorks.  Your profile defines a tolerance zone that allows anything from a sharp corner to a 17.66mm radius.

   I recommend a ± tolerance on the radius.

   Your zero point specification looks weird, and unlike anything I have seen in ASME Y14.5.  

               JHG

RE: Bend Radius Tolerance

twkinfected ... interesting moniker.

Anyway, your interpretation is correct.  Bend radii are more commonly toleranced directly with +/- unless the bend itself also has to nest with a mating surface.  Depending on stress concentration issues, etc, you may want to make it a CR (controlled radius).

I'm in accord with Kenat that the GD&T overall is badly done.  Datums B&C are not valid because they don't invoke the boundary, but rather just the radius; i.e. it's not really a feature of size other than at the tangencies.  This looks like an adjustable corner bracket; more typically the face perpendicular wrt datum-A would be called out as the secondary datum feature and the length would be called out as the tertiary datum feature of size.  Then, the holes & edges & such would be located wrt those datums.  Lots of assumptions on my part, but the part looks just like a corner bracket for securing a table top to the skirt trim, with lots of adjustability designed in.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Bend Radius Tolerance

I see, it's the aspect not covered by 'simplistically' that you're questioning.  You're right, since the profile also allows shift of the location of the radius as well as it's size you could get a small rad pushed into the corner.

This would be allowed per my understanding of the drawing.

It may not be what was intended if they were trying to prevent cracking etc.

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"?

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