PDA

View Full Version : Metric Drawing Help



ERBenoit
07-07-2008, 05:46 PM
I do not do a lot in metric :mad:, when I have to, I turn it into inches. I need some help deciphering fit class information this section of a metric :mad: drawing. It is a masking plate for a punch cutting die. Two 6 mm dowel pins, locate on two holes (other not shown) to align the plate with the die. I do not have the drawings for the punch part of this cutting die.

http://i351.photobucket.com/albums/q471/2006-6002/Part.jpg

The 6mm hole/bore "G5" in particular. I find no information on what tolerances apply to "G5". Or are the tolerances right there in plain sight as the +.004 +.009 assuming mm, in parentheses following the "G5"?

If this drawing were in inches I know what the +.004 +.009 means, in mm that difference is roughly .0002". Is this telling me that the clearance for dowel pins for this die plate is only .0002"? IMO, too close a fit in this application.

I find "G7" and "g6", but no "G5". The only thing I can find in Machinery's Handbook that are relatively close (and that is only because I find a "g" from the ISO Symbol) is:

"H7/g6 G7/h6" which is noted as a "Sliding Fit -- not intended to run freely, but move and turn freely and locate accurately." In this application nothing is running or turning.

But:

"H7/h6 H7/h6" which is noted as "Locational clearance fit provides snug fit for locating stationary parts; but can be freely assembled and disassembled."

"H7/k6 K7/h6" which is noted as "Locational transition fit for accurate location, a compromise between clearance and interference.

I cannot accurately measure the dowel pins due to thier location, so I am having some difficulty in determinining which of the above fits best suits the application as shaft, in this case the dowel pin and hole diameters determine the classification of the fits. They all, to some degree seem suitable. Though by description, sliding fit and locational clearance seem to be the best.

SDL
07-07-2008, 06:46 PM
Your understanding is correct if you go to here

http://www.mecc.polimi.it/~giglio/machine%20design/Practical%20exercises/ISO_Tolerance_Part_2.pdf

and scroll down to page 17 of the pdf file you will see tolerances are as on your drawing.

If you look at page 8 figure one you will see that G tolerances are above the nominal line, most of the time people are used to the H class.

Steve Larner

juergenwt
07-08-2008, 01:33 AM
6G5 hole = +9/+4- in inches +0.00035/+0.00015
Only a person not familiar with metric dim's or some body that does not know what he is doing could have put these dim' on a print.

The proper dim's for a dowel pin would be 6 H7 (0/ +8) for the hole and a standard dowel pin 6 m6 (+4/+12)for the pin. Use a standard 6 H7 reamer and a standard 6 m6 dowel pin.

The guy who put those dim's on should be charged for jig grinding to those tolerances and than his boss should fire him or send him back to school. You will be just fine with the tol. I gave you.If he wanted an absolute press fit he should have a 6 H7 hole and a 6 s6 pin. But I do not think that is what he wants.He just wants a plain old dowel pin for location. These are errors made mostly by people having no experience working or thinking in metric.Juergenwt
PS.:One more thing. What kind of steel are you using? Toolsteel will usually stay the same or the holes would get slightly larger. So if you use a brand new 6 H7 reamer take a small piece of steel and drill and ream a hole to make sure you have a tight fit for your dowel. Slow speed and lubricate. If you have to, take an oil stone over the reamer edge-lightly.
For case hardening steel - the holes will shrink a small amount and you may have to lapp ore hone.