Sheetmetal Channel Concentricity

[TomFin]

Hello All,

I have a flat pattern with two symmetric holes that will be bent into a symmetric channel thus making these two holes concentric.
As far as the drawing I'd like to specify the two holes as concentric. From my understanding, to accomplish this I'd have to assign one of the two hole axes as a datum then reference this datum at the other hole with a concentricity call out.

Is there a better or more clear way to convey allignment of the holes ?

Thanks in advance

Failure is a prerequisite of successful design

 

[PaulJackson]

Tomfin,

It is near impossible for a single hole in sheet metal to create a stable, repeatable axis for measurement all by itself. Typically the depth of the cylinder is too shallow. Therefore if you did declare it as a primary datum feature to check the location of the other coaxial hole inspectors gage-makers, etc. would "choose" something else on the part that makes sense to them to serve as a primary (stopping rotational degrees of freedom) and then they treat the hole as a secondary datum feature establishing a X0,Y0 reference at its axis (stopping translational degrees of freedom). The point is that if the GD&T renders an unstable or unrepeatable measurement system most will substitute it for one that makes sense to them and is stable.

To determine what should serve as primary, secondary, and tertiary datum features for the part you should always examine its function. What physically and functionally on the part removes rotational and translational degrees of freedom? Say for instance that the two coaxial holes have a long bolt that goes through them in the assembly and the axis through the two holes actually determines where the sheet metal surfaces end up in the assembly. If that was the case the functional primary datum for the part would be the axis of the two coaxial holes (removing 4 degrees of freedom), say the secondary was the width between the thrust surfaces adjacent to each of the coaxial holes (which stops translation along the axis) and the tertiary what ever functionally stops rotation about the axis.

If that system represented function and was stable and repeatable there would be no reason for an inspector or gage-maker to consider an alternate method to check the part.

Now to answer your question, if the sheet metal surfaces align and locate the part in the next assembly and the hole locations are dependent upon where the surfaces put them then give the holes location tolerances from that sheet metal surface coordinate system and size the holes so that given thier location tolerance for not being coaxial, whatever has to pass through them will function.

If the the holes themselves are the functional primary datum and you want to tolerance their coaxial orientation toward one another Call one |A| one |B| and tolerance the location of "A"@ MMC to |A(M)-B(M)| likewise for "B". Then tolerance the adjacent thrust surfaces for squareness to the primary datum axis.

The point is whatever the parts' function reveals how the part is oriented and located in the next assembly USE IT! (if possible) to define the tolerance zones for functional variation of the parts contour.

Paul

 

[KENAT]

Paul, am I correct in assuming that in the case you've assumed by location you mean to use a Positional Tolerance?

This was how I was thinking but am not as well educated/experienced and was having trouble getting my head around the positional to the axis of holes A & B.

To the OP, while simplistically you may be wanting make the holes concentric, in Practice 'Concentricity' is rarely the correct control.

As Paul says function should drive the GD&T. If simplistically the holes need to line up to let a bolt or something go through then position may be the way to go.

KENAT, probably the least qualified checker you'll ever meet...

 

[PaulJackson]

Kenat

It would be silly for me or anyone else to recommend the best method to tolerance the location or relative coaxiality of the two sheet metal holes without understanding what the functional purpose of the holes are. Failing that we can only imagine what-if scenarios.

I understand your advice and reservations concerning the use of concentricity but I thought that was less of a problem than what I imagined “Tomfin” has to deal with in-terms of the specification and its outcomes in measurement. Using one sheet metal hole (and possibly other unspecified datum features) to establish an axis and then project that axis a considerable distance to check the location of another sheet metal hole would typically produce wildly varying measurement results. Those results would have little or no value in determining the location of the latter hole or its effect on coaxiality of the two holes. I imagine if the pair of holes were not the primary functional datum feature that it would be better to just tolerance each hole’s location independently or as a pattern from the functional sheet metal surface datum features.

I the two holes were the functional primary datum feature then tolerancing their coaxiality is a housekeeping control that unfortunately should be present but is a problem because of its difficulty to quantify. It can however be checked fairly simply with an attribute gage that looks exactly like a shaft or a long bolt if the position tolerance was set up as I mentioned earlier. Dia A |pos|dia 0(M)|A(M)-B(M)| and Dia B |pos|dia 0(M)|A(M)-B(M)|.

Paul

 

[KENAT]

Agree Paul giving detailed recomendations without understanding function etc is unwise.

I was just trying to make sure I understood what you'd put for my own selfish reasons.

KENAT, probably the least qualified checker you'll ever meet...

 

[TomFin]

Thankyou PJ for the elaborate and thorough explanation. This set of holes is one of two sets with equal importance in terms of functionality. They are basically clevises for pins. I also agree that gd&t is requires upper assembly level knowledge and there is no cookbook for applying symbols which is why I appreciate both of your exchanges. I feel that a positional tolerance akin to functional allowance is the best route.

Rant...
Our mfg plant has never embraced GD&T. The shop, both inspection and fabrication wouldn't know a positional tolerance if they saw it and would just ignore it. The scary thing is I've seen a lot of drawings at our shop plagued with improper concentricity callouts which is why I posted. It almost seems as though the drafters are aware of the shop's indifference to "advanced" symbology. So drafters place concentricity callouts without datum references for the shop to interpret as "Make sure these holes lineup somewhat so assy doesn't have to use Thor's hammer." Now that my name is on the drawing I'd like to properly specify these drawings just in case the big dogs ever decide to train the shop properly.

Failure is a prerequisite of successful design

 

[dingy2]

Do not use concentricity. It is not applicable here.

I would agree that positional tolerances are more appropriate but you must develop our datum set up.

Good luck on this one since the shop floor would ignor it anyway.

Dave D.

http://www.qmsi.ca