What's new
What's new

.050r max

TiTillIdie

Plastic
Joined
Aug 27, 2015
This should be a simple question, but it seems as we have a slight discrepancy in the way a print calls out a radius. If a print says .050R MAX, could it be 0? To me, anything under .051 should be acceptable. even if it is 0.
 
That's the way I read it, although I usually put some kind of radius. Usually whatever tool I have that has a radius under .050 that way I don't have to buy anything special.
 
Dumb ass engineers and production design people come up with more stupid dimensions and tolerances
 
likely worried about Interferences in corner .. I have seen that often on grinding part prints.

QT: [anything under .051 should be acceptable.] perhaps with +- .001 or +- .005 on some prints... *but I would not take the chance for argument and hold .050 and less...
 
This should be a simple question, but it seems as we have a slight discrepancy in the way a print calls out a radius. If a print says .050R MAX, could it be 0? To me, anything under .051 should be acceptable. even if it is 0.
Zero is nothing. If it calls for a radius, and you give it zero radius, there is no radius. The part is wrong.
 
A sharp corner satisfies 0.050R MAX. Sharp inside corners are not good ideas, but it's the customer's job to specify the tolerances. As michiganbuck said, this is almost certainly to ensure that this part and some other part will seat properly without interference.
 
Whoever "designed" it doesn't want a sharp edge so any small radius under 0.05 is OK. A small chamfer would/could also be regarded as having sharp edges.
 
There is no min spec. and you can't make a "zero" anyways.
You are correct. Anything below .050 plus whatever the tolerance block gives.
Bob
I disagree. Title block tolerances are for stuff not otherwise specified. ".050 Max" is specified, therefore title block tolerances don't apply. No?
 
This should be a simple question, but it seems as we have a slight discrepancy in the way a print calls out a radius. If a print says .050R MAX, could it be 0? To me, anything under .051 should be acceptable. even if it is 0.

This is making a mountain out of a molehill. An R is stated and this means a radius. What is called for is a radius no larger than 0.05. Sharp edges and chamfers are not radii.
 
Is the drawing per ansi y14.5 or asme y14.5? A "R" is a boundry and any shape inside the boundry is acceptable excluding reversals. A "CR" is a controlled radius and must be a fair arc with radial control.
 
Is the drawing per ansi y14.5 or asme y14.5? A "R" is a boundry and any shape inside the boundry is acceptable excluding reversals. A "CR" is a controlled radius and must be a fair arc with radial control.

I don't doubt that you're correct but the drawing probably didn't reference any standard. I can't help but think that R.03 ±.02 would have solved all problems.
 
Perhaps good to hand hone break the cutter corner about .000012 if that is a concern to producing the job. We would leave the corner .050 to zero radius for grinding parts and never got a job back. Most often to 3/64 or less (to zero) just to save the time of checking on the shadow graph. Yes grinding is different because it is near impossible to get a dead sharp corner. Adding a .005 radius would often include a wheel change , face and OD dress, blue-up, hand feel the floor of the part. slow come-in and careful watching. likely a 1/4 hour addition to part cost. Yes a dressed radius would not be performed, just going to the smaller grit wheel would get the desired smaller radius.

Even employing that hand hone bump to the end mill might defeat the designers purpose of saving the time and additional cost of adding a radius to the part..The cost of a special .025/,030 radius end mill might be $100 or so, add a tool change, tweak the extra pass into the program, hold the job up three days to consult the PM guys, give you dog a dirty look because of being upset, loose a nights sleep in worry,
 
My take is a sharp corner meets spec. Max is max. I do run into the used of max and min where it does not work correctly. usually min. If min. then the part would not have a shoulder as an example. Now if they needed a radius for stress relief, then they could spec in and under cut radii.
 
I'm also in the camp of "Sharp to .050 R is acceptable". I have ALWAYS interpreted this specific designation, not as a feature specification per se, but an allowance for configuration based on shop options, tooling at hand, and designer's functional requirements. I don't think that because it says "R" that a radius is being mandated. And as Larry Dickman notes, this type of note is often used to indicate intent of sharp corner in the context of ".005R max". When the nomenclature "CR" is used, that IS a specification for a radius.
 








 
Back
Top