Dimensioning Interpretation

[Eins73]

Hi All,

Need help to understand chamfer function and how to read it. for example, I got a ch0.05 indicated on a corner. No tolerance given and general tolerance is +/-0.15.
1)does this general tolerance implies to chamfer dimension
2) with the general torences, can the chamfer be avoided

TQ

 

[powerhound]

Answer to #1: Yes, unless there is a note that specifically applies to chamfers.
#2: Probably not.

In all likelihood, it was probably an oversight on the part of the drafter. If asking the customer is not an option, I would just put a chamfer there as close to .05 as I could and if I catch any grief for being a little over or under, I would point out the fact that per the print, the chamfer didn't have to be there at all.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Eins73]

If I to put the dimension, it will be ch 0.05 +/-0.15 (which is, tolerance>nominal). doesn't it indicate a negative chamfer dimension

 

[powerhound]

Well, in reality, there's no such thing as a negative chamfer so you won't have to worry about that happening. It's not all that uncommon for drafters to apply dimensions without thinking about the implication of the general tolerance block. Seriously, just put a .05 chamfer there.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Eins73]

this is a problem I encounter with vendor when they fail to produce that 0.5 chamfer. This non-chamfer side cause a defect in my part. I would say that this is also a design issue. better to be : ch 0.5 min

so, thank you John

 

[pmarc]

If from design perspective MIN value of chamfer is desired, I would say this it is not design issue, but drawing specification issue.

Even a worse thing can happen. I have seen manufacturers claiming that according to 0.05+/-0.15 a burr instead of an undercut is acceptable (see attachment). They hold to this interpretation especially when they realize that they omitted or were not able to produce a chamfer and they need an excuse. In my opinion, looking objectively, despite they did not do their job well, there is no reason to say they are wrong.

http://files.engineering.com/getfil...b-a834-aaf7a21f95a3&file=undercut_vs_burr.png

 

[CheckerHater]

If we are seriously considering worst case scenario dealing with Bad Guy Supplier, using MIN implies that there is no upper limit, so chamfer can be infinitely large.
If OP wants to rely on default titleblock tolerances the best way is to separate, something along those lines:
UNLESS SPECIFIED
SIZE TOLERANCES +/- 0.15
CHAMFERS +/-0.025
Or just tolerance the chamfer directly.

 

[powerhound]

Yes, it is a specification issue. So it sounds like you are the one who overlooked the relationship between the specification and the general tolerance. Also, I assume you still mean .05 instead of the 0.5 that you are now saying.

pmarc, I have also seen the scenario you presented. Most times it is exactly as you say, they just forgot; however, I have had the discussion about whether or not to deliberately leave a chamfer off if it is still within spec AND it speeds up the process. Granted that may not be the right thing to do, but it's exactly why drafters should be meticulous in what they do. A drawing should close any loopholes. I've spoken to countless engineers who say that if any shop gave them a part they couldn't use because they didn't follow "Industry Standard" then they would never use that shop again. My answer is always "How does that help you right now with these 1000's of dollars worth of useless parts you have to buy?"

To CHs point. He's exactly right. You have to be careful how you deploy MIN and MAX values. MIN means no maximum value and MAX means no minimum value. That is explicitly stated in the ASME Y14.5 standard.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[looslib]

The bst way to avoid confusion is to limit tolerance the chamfer: 0.05-0.15
You have your minimum, you have your maximum, no burr overhangs, no sharp edges, no skipped chamfer because a 0.0 chamfer was within spec range.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[ewh]

I prefer Ben's suggestion. If there is a design requirement, document that requirement.
I recently had a similar discussion here at work regarding the standard dwg title block, which contains the statement "BREAK SHARP EDGES .015 MAX."
When I pointed out that the statement actually allowed relatively sharp edges I received a variety of responses... "edge breaks are required in the work instruction", "why would a vendor bother to break an edge .001?" "it would raise cost and affect non-conformance", "we don't care how small, as long as it is there" to my favorite "we don't inspect those anyway". It actually boiled down to TTWWADI.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[dgallup]

If a relatively sharp edge presents no problem then I will just draw the edge sharp and use a standard title block note for the maximum break edge permitted. We also nearly always have an additional note about burrs such as "NO VISIBLE BURR AT 5x MAGNIFICATION". So that prevents a truly sharp corner or burr. If the chamfer has to have minimum and maximum values and/or a specific angle for functional or assembly reasons then it becomes a feature with dimensions. I would never give it a tolerancing scheme that would allow a zero or negative chamfer.

For the OP, I would second powderhound, the general tolerance applies but there has to be some (perhaps microscopic) chamfer because it is a feature called out on the print.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.