Profile Tolerance regarding to other profile as Datum
Profile Tolerance regarding to other profile as Datum
(OP)
Before anything I have to say that I am beginner in GD&T, and it is really interesting, I am a mechanical designer and recently I have designed some components for certain stamping process, as you understand accuracy is critical and some surfaces must be controlled using profile tolerance, to illustrate the situation, attached you can find a PDF drawing with one of the components which I recently have designed, In this component the outer profile should be controlled as is stated, but I have an other very important profile(showed in “Detail B”) which shall be controlled by the profile represented by “DATUM D”, and it has to be controlled all around by this boundary. I am not sure if this kind of tolerance is correct, or even if will be interpreted as my intend.





RE: Profile Tolerance regarding to other profile as Datum
KENAT, probably the least qualified checker you'll ever meet...
RE: Profile Tolerance regarding to other profile as Datum
RE: Profile Tolerance regarding to other profile as Datum
Heckler![[americanflag] americanflag](https://www.tipmaster.com/images/americanflag.gif)
Sr. Mechanical Engineer
SWx 2007 SP 4.0 & Pro/E 2001
o
_`\(,_
(_)/ (_)
This post contains no political overtones or undertones for that matter and in no way represents the poster's political agenda.
RE: Profile Tolerance regarding to other profile as Datum
KENAT, probably the least qualified checker you'll ever meet...
RE: Profile Tolerance regarding to other profile as Datum
Since the feature is asymetrical, there needs to be a tertiary for anti-rotation.
I would say fix the datums and then let's look at the profiles.
Dave D.
www.qmsi.ca
RE: Profile Tolerance regarding to other profile as Datum
I’d perhaps make your datum D into datum B and use the flat produced by.2972 as C if you need orientation. Datum selection needs to be based on function though which I don’t fully know.
Take a look in 14.5 at section 6.5. Figure 6-17 is vaguely similar to yours.
I don’t think you need the composite frames.
KENAT, probably the least qualified checker you'll ever meet...
RE: Profile Tolerance regarding to other profile as Datum
Briefly, how is this insert used, or installed in subsequent operations please?
RE: Profile Tolerance regarding to other profile as Datum
That being said...
alrayo,
Get rid of the datums on those centerlines, change datum D to datum B and make datum C the flat on the left side of the part in the top view. Redefine your datum reference frames on your profile callouts as necessary. If you use composite profile, each segment must have a datum reference, unlike composite position.
Once you have that done, repost a drawing for us and we can give you a little more help.
Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
RE: Profile Tolerance regarding to other profile as Datum
RE: Profile Tolerance regarding to other profile as Datum
Looking better. Some things to be considered: No need for the 'CL' on centerlines. Need a class designation for the thread callout. The Datum C definition is "troublesome" IMHO and does not go well the datum C in the FCF. A few other that the checkers should pick up on.
I assume that you have a checking group which will review your new results.
RE: Profile Tolerance regarding to other profile as Datum
You need to have a datum reference in the lower segment of your composite profile. What message are you trying to convey by the lower segment when the value is exactly the same as the upper segment and there is no datum reference? What are you trying to say when you put BOUNDARY below the datum B identifier? You don't need the reference to datum C in your FCF that controls all those countersinks.
On your print of the mating part in sector C8...the parallel and profile tolerances overlap each other. You can get rid of the parallel because the profile of a surface referenced to A controls the parallelism within the tolerance zone of .0002.
Back to the first print; if the sole purpose of those countersinks on either side of the tapped hole is just for lead-in for the bolt, I don't think I would call it out so tightly. As it is, all untoleranced dimensions are basic per your note so you would need to further define the countersinks with a geometric tolerance. You should really pore over your drawing to make sure that all the dimensions that need to be toleranced are done so. I don't think you intend for that counterbore to have a profile of .0003 applied to it. Double check your reference to surface finish in note 2 versus the statement in the upper left of your title block. You have a .125 hole called out at .360 deep. Elsewhere in the print, the same hole is shown .358 - .362. You can't do it like that. Someone will make that hole .360 deep +/-.005 and you may have to buy that part anyway if it's .364 deep.
Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
RE: Profile Tolerance regarding to other profile as Datum
A question with regards to Datum B. What is the true geometric counterpart of datum feature B as currently indicated? If it is as I think, what is the benefit or need for C?
Kinda complicated aint it..
RE: Profile Tolerance regarding to other profile as Datum
Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
RE: Profile Tolerance regarding to other profile as Datum
I for one would like to see the final results of your drawing after review by your checking group. I imagine that others might like to see the same. Is that a possibility?
There are a lot of little issues that should be addressed,
but not yet mentioned my anyone. Self included.
RE: Profile Tolerance regarding to other profile as Datum
Other issue will be the matting process between the “Inner insert” Vs “Pre-Curl Die”, I have invoked the section 6.5.5.1 (Boundary Control for a Noncylindrical Feature) to define the tolerances to apply on this two components.
RE: Profile Tolerance regarding to other profile as Datum
I applaud your persistence to get this right. As mentioned by ringman, there are other standard related issues that indeed need to be addressed on both component specs. But first to best help you, I/we need to further understand the function and the assembly sequence/process of the insert to the die. More specifically the two threaded (5/16-18-2B) holes, datum C on each component. Could you please elaborate?
RE: Profile Tolerance regarding to other profile as Datum
"X.XXX REF." is not preferred, having been replaced with "(X.XXX)". The period is also not needed, unless the abbreviation can be confused with another word, such as "no" and "no.".
"THRU" is not necessary if it is shown in a view as being through the part.
The "S" modifier is now obsolete; if "M" or "L" is absent, "S" is inferred.
"...TAP..." is specifying a method - Only the thread callout is needed.
You don't need to specify "POLISH" with a 4 finish; however it is achieved, it will be "polished".
A countersink is inferred to be nearside unless specified otherwise.
These are not usually considered major issues, but can go a long way towards de-cluttering a drawing, which in turn makes it easier to interpret, thus less expensive to manyfacture in the long run.
Are you limited to one sheet B size dwgs? Breaking these views onto multiple sheets would also go a long way towards simplification.
Keep up the good fight!
RE: Profile Tolerance regarding to other profile as Datum
Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
RE: Profile Tolerance regarding to other profile as Datum