Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • 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!

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

Donate Today!

Do you enjoy these
technical forums?
Donate Today! Click Here

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

Jieve (Mechanical) (OP)
30 Apr 12 20:37
Hello again,

Couple more ISO GD&T questions:

1) Assume I have a disc 220mm in diameter and 25mm thick that will be rotating at speeds up to 2000RPM. The center of the disc has a hole 38mm in size and is mounted on a hub. On the drawing for the disc, I specify datum A as a flat face of the disc and datum B the center axis specified by placing the datum symbol on the outer diameter. If I were to specify a position control tolerance of the center hole with respect to the center axis of the disc of 0.1mm as well as a total runout tolerance of the outer diameter of 0.1mm with respect to the inner hole (axis), is this redundant? It seems to me that if the position of the hole is off by 0.1mm then the total runout would be off by at least this much as well. Would it be better to simply call out a total runout tolerance and control the perpendicularity of the center hole with a perpendicularity control?

2) Assume I have a rectangular part with 3 pegs, and a mating rectangular part with 3 holes (the pegs fit in the holes). Both rectangular parts are the same size. I am more interested in the pegs fitting together than I am of their relation to the edges of the part. On the part with the holes, I choose the primary datum to be the face perpendicular to the hole axes, and two sides to be datums. I then specify a position tolerance of the holes of say 0.2mm, and I refine that tolerance with a dual position frame to 0.05mm with respect to datum A to keep the hole tolerance zones locked together. If I were to apply position tolerances at MMC for both the holes and pegs as well as 0 perpendicularity tolerance at MMC, would it then be best to specify the same tolerances with respect to datum features that are coplanar with the secondary and tertiary datums on the part with the pegs? In other words, should the hole/peg patterns of such mating parts be given the same position tolerances from the same (coplanar) sides of the parts?

3) Assume I have the rectangular part with the holes as mentioned above. If I specify a position refinement tolerance (second position control under an existing position control) for a group of holes, only specifying the primary datum A (perpendicular to the axis of the holes) without reference to any other datum, can the pattern still rotate with respect to the secondary and tertiary datums, or can it only translate?

4) When selecting datum features for discs with holes through the center, such as in my first question, is there a rule of thumb or are there maybe specific common applications that warrant having either the hole diameter or the disc diameter take precedence over the other as a datum feature? As the parts need to be mounted on these datum features, it seems that certain parts may be more easily mounted on the inner diameter, but I'm assuming this selection should be based on function more than on mounting considerations. Just curious if it is more common to use, for example, the inner hole feature for rotating parts, etc.

Thanks!   
pmarc (Mechanical)
1 May 12 6:07
1) & 4) - From functional point of view the inner hole seems to serve much better as a secondary datum feature. If the disc is mounted on the hub, the inner hole mates with it and stops 2 translational degrees of freedom, not the outer diameter. Having said that, I would most likely recommend defining perpendicularity tolerance of inner hole's axis relative to datum plane A (if you are not OK with those wicked title block angular tolerances), attaching datum feature symbol B to that perpendicularity FCF and put runout tolerance relative to A|B for the outer diameter.

And answering to your question about potential redundancy of your tolerancing scheme, no offence, but I would call it slightly illogical. (I am not thinking here about values, but about datums selection). First you choose outer diameter's axis as a datum for position of hole's center and then suddenly you pick inner hole's axis as a datum for runout of the outer diameter. What is the reason behind it?

------

2) In case of simple rectangular blocks with series of holes/pegs, I would probably assign the same (corresponding) planar features as secondary and tertiary datum features and most likely apply the same values of positional tolerances. Though I would be careful treating it as a rule of thumb in case of more complicated parts.

You mentioned something about 0 perpendicularity at MMC. Are you going to use it in lower FCF's for holes and pegs as a refinement of upper position callout? If yes, be aware that it will not not control spacing between holes, which would be controlled if position symbol was there.

Out of curiosity, what are the size limits for pegs and holes that are going to be assembled? And is this going to be a loose fit or something with interference?

------
  
3) Yes, the pattern can still rotate with relation to datums B and C. Having only A referenced in the second FCF means that pattern of positional tolerance zones is perfectly perpendicular to datum plane A and the zones are perfectly spaced to each other, but says nothing about orientation of the pattern relative to datums B and C. If you need orientation constrained, you have to add second datum reference (B or C) to the FCF. Just keep in mind that this will also tighten location of the pattern relative to that referenced secondary datum.
fsincox (Aerospace)
1 May 12 12:35
Before the release of the ASME 1994 standard we would add a flag note to composite tolerances stating: "datums restated for pattern orientation only". Georg Henzold (ISO book)  has just a "*" next to the restated datum and then a note "* orientation only".
Frank
pmarc (Mechanical)
1 May 12 14:05
Frank,
If I correctly understand what you mean, there is a new modifier introduced by ISO 5459:2011 "><" which means "for orientation contraint only". I think it finally opened the door for having meaning of ASME composite positional tolerancing covered by ISO GPS operators.

An ISO positional callout for pattern of at least 2 holes relative to typical datum reference frame structure derived from 3 mutually perpendicular planar datum features...:
|Pos.|dia.0.8|A|B|C|
|Pos.|dia.0.2|A|B><|
...is in my opinion of the same meaning as ASME composite:
|Pos.|dia.0.8|A|B|C|
|      |dia.0.2|A|B|  
Walterke (Industrial)
2 May 12 3:57
Small suggestion:
In stead of a page long description of your problem, why don't you just make a quick drawing of it?

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

fsincox (Aerospace)
2 May 12 8:26
pmarc,
That will do it then, thank you.
Frank
Jieve (Mechanical) (OP)
2 May 12 18:00
Pmarc, thanks again for the answers.

With regard to the rotating disc, you're totally right about having a runout and position in the way I described being illogical. Actually, On the drawing i submitted to the shop, there was only a position tolerance of the center hole with regard to the outer diameter with no total runout callout. The more i thought about the application though, the more it seemed that a total runout would be better. I have revised the drawing using the inner hole center axis as the secondary datum, eliminated the position tolerance and controlled the perpendicularity of the center hole with a separate callout, then added a total runout tolerance to the outer diameter with respect to the inner.  Interesting that you say the runout tolerance should include the primary datum A (flat face) as well.  I'm envisioning the person inspecting the part mounting the inner bore On a precision spindle and simply measuring the runout similar to how the part will be mounted during normal application. Why should i include the primary datum in the runout?

My second question about the pegs and holes was actually more of a thought question, not directly applicable to any of my parts. I remembered reading in a textbook about dimensioning mating parts that the dimensions should generally be from the same "side" of each of the parts but was wondering if this changes based on the use of GD&T with position control callouts.  In the application I was thinking of, the holes were clearance holes. But now that i think about it, how would you deal with this Situation if the pegs were interference Fit? Seems like you'd need extremely tight position tolerances to have more than one peg interference fit in a mating part.  
fsincox (Aerospace)
2 May 12 19:45
pmarc,
Is it literally "><" as shown?
Thanks,
Frank
pmarc (Mechanical)
3 May 12 10:23
Frank,
Yes, it is >< after datum letter within FCF.
fsincox (Aerospace)
3 May 12 15:52
pmarc,
I wanted to check to see if it was a symbol error.
Thanks,
Frank

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!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close