"In line" tolerance?

[handleman]

I'm dimensioning a weldment part (picture attached) that has a couple of H7 toleranced dowel pin holes for alignment of a linear guide component. The component has a datum edge that will be "bumped up against" two dowel pins in the H7 holes before being tightened down with screws into the four tapped holes. If it matters, this is for a piece of one-off equipment, so only one of these parts will ever be made. I don't really care at all about the absolute position of the holes in the face, but I do want to make sure that the two H7 holes are "vertical" to one another with respect to the bottom surface, so that when the bracket is assembled to a base plate the linear motion component will be vertical. My supervisor told me to just draw a dimension/extension line between the two hole centers and specify perpendicularity between that line and the bottom surface. While that does seem to communicate what I really want, I (think) it's totally wrong. How can I tolerance this part without adding a bunch of unneccessary cost?

Thanks!

-handleman, CSWP (The new, easy test)

 

[KENAT]

I'm wondering if you could use a composite position on these holes.

Relatively loose for overal location then tighter as a pattern, with the 'lower' part of the FCF referencing the relavant datum to give the 'vertical' control you need.

Maybe the lower half doesn't even need to use diameter position, just 1D wrt the relevant datum, but I'm not totally sure this works.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at

http://eng-tips.com/market.cfm?

 

[Tunalover]

A better way is to assign a datum to one hole then give the second hole a positional tolerance using that datum as the primary datum. As long as the first hole is toleranced so it'll be as you want it the second hole will be very coaxial if you keep the positional tolerance small.


Tunalover

 

[handleman]

I don't care a whit about the absolute position of either hole. I just want the axes of both holes to "pierce" a line that is perpendicular to the base.



-handleman, CSWP (The new, easy test)

 

[axym]

I think Kenat is on the right track here. A loose position tolerance on the pattern, referencing the "front" face, the "bottom" face, and some other datum for left-right location. I realize that absolute location is not important, but it has to at least be in the ball park.

A tight position tolerance on the pattern, referencing the front face and bottom face, would give the desired "verticality" control. If a composite FCF was used as Kenat suggests, the tolerance zone pattern would be oriented relative to the bottom face datum but not located relative to it. Which is good. But the lower tier would also tightly control the spacing between the holes, which is not necessary in this case.

This could be relieved by using a bidirectional position tolerance on the pattern instead of the composite second tier (again refencing the front face and bottom face datums). A tight tolerance in the horizontal direction will give the desired control, and a loose tolerance in the vertical direction will give the desired relief.

There is usually a way to encode the exact control that you want, but the drawing may become very complicated. You'll have to weigh the value of the potential manufacturing cost reduction against the possibility of confusing the heck out of whoever's making the part. Oh well, that's part of the wonderful world of GD&T!

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[handleman]

There is usually a way to encode the exact control that you want, but the drawing may become very complicated. You'll have to weigh the value of the potential manufacturing cost reduction against the possibility of confusing the heck out of whoever's making the part. Oh well, that's part of the wonderful world of GD&T!

That's certainly a valid point! In our case, since we usually make just one of any part (rarely is any part qty over 5), the benefit of using a complicated GD&T scheme to "loosen up" the tolerances to the minimum requirement would have been pretty small. Many shops that we use would glance at the drawing and quote it high due to the complicated GD&T. This part was only qty 1. I had to release the drawing the day after my original post.

I know that purists are gonna cringe, I complied with my supervisor and put a perpendicular tolerance on a line drawn between the two hole centers.

-handleman, CSWP (The new, easy test)

 

[ewh]

The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]

 

[powerhound]

I think the answer would have been use a single segment positional callout. You know, the one that's like composite except instead of having one position symbol for two lines, there's one symbol on each line. This way you can move the pattern around per the PLTZ but the features remain basically located to whatever datum you decide will be perpendicular to the base. This allows you to tighten up the tolerance left to right without tightening it up vertically.The callout advised by your supervisor is illegal per the standard. Orientation (perpendicularity in this case)controls individual features, not imaginary lines between features as you have shown on your drawing.
Sorry for being late with this.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ringster]

It appears that the 'in line' reference is in error. It sould seem to be a parallel relationship that you are looking for. Maybe someone can provide support or contradiction for that opinion. Hopefully support.

 

[powerhound]

Parallelism is also an orientation control and thus would not apply here. You can specify a feature parallel to a datum using parallelism but not to an axis between a group of features. You might be able to add a note to verbally express your intent but then that would negate the point of using a symbol.

I really think that two single-segment FCF's as represented by the 5mm diameter holes in Fig. 5-21 is what you're looking for.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ringster]

H7 holes are "vertical" to one another with respect to the bottom surface,

The way that i read this is 2 axis perpendicular to a plane are therefore parallel to one another.

IS there something that I have missed.

 

[powerhound]

Your first sentence kind of makes sense when typed out. The challenge, however, is to convert that thought process into a legal GD&T specification along with applying the desired tolerances.

I don't understand your second sentence though because the axes of the holes are actually parallel to the bottom plane. What you probably meant to say is that an imaginary line drawn between the centers of the holes, along the same plane, should be perpendicular to the bottom plane. This imaginary line is not a feature nor an axis and thus cannot be controlled by GD&T, only features can.

Lets say there was only one H7 hole in the face of this part. Would using the perp callout be appropriate? No, because there's nothing perpendicular about it. It is simply a hole above a plane. Adding a hole to the situation does not change this. Axes and planes are not controlled using GD&T, features are. Axes and planes are determined by the feature, not the other way around.

It may just be a matter of thinking about controlling what is there instead of what isn't there.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[aardvarkdw]

Powerhound,

I just had this exact same situation come up today and after reading through the standard I fully agree with you and used the stacked positional tolerance FCF's as shown in fig. 5-21

This is exactly the situation that composite tolerances were designed for.

David

 

[ringster]

...sure that the two H7 holes are "vertical" to one another...

I reread the OP and just noticed that it requires the H7 holes to be vertical to one another. I believe the post should be rewritten to properly describe the problem. I dont believe that this expresses the 'real intent'.

 

[handleman]

Well, then, why don't you go ahead and rewrite the post for me?


-handleman, CSWP (The new, easy test)

 

[ctopher]

Make the side of the part perp (some tol) to the mtg surface. Then dim (basic) the two holes to the side surface.
Or something similar.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[powerhound]

I think if we would have been on the wrong track, handleman would have said so. His drawing and his post were clear to me and the others that answered his post. I don't think the reason for your misunderstanding is in the OP.
As I said in my original response to you, your first sentence actually made sense, so you seemed to have understood the OP and that point, what happened?

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[handleman]

Chris,
That is exactly what I would normally have done. However, I was trying to avoid adding controlled surfaces that weren't necessary for the final function of the part. Plus the tolerance stackup involved.

At this point it's all an academic exercise, since the drawing has already been issued, the part fabricated, and assembled in a piece of machinery. It's kind of funny that all the activity (KENAT's timely response excepted) in this thread began exactly a month after my original post. Not that I'm complaining or "expecting" service as though I'd paid for it, just kinda funny. Threads usually die after languishing for more that 3 or 4 days.

Thanks, everybody!

-handleman, CSWP (The new, easy test)

 

[aardvarkdw]

Would you believe it. I just got told to remove the FCF's from my print and replace it with ± tols. because the tols didn't need to be that "tight". The joke is that the GDT was actually a LOOSER tolerance than the one I was told to spec! After asking about this and explaining what was intended, I was essentially told that the we didn't want to confuse the shop... They pay me to do it their way though so I wont push the issue.

David

 

[ctopher]

Must be the purchasing dept involved.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion