controlling bow of part in one direction

[Kinsrow]

I have a plastic injection molded part that is .120" with +/-.004 and flatness call out on the bottom surface of .010". To me this doesn't make sense. Anyway, what I'm trying to do is to control the thickness and the direction of the bowing. I would rather bow in one direction so that it will be flush to the mating surface when assembled. the length is 6 inches and width is say .25". what would be the best way to dimension this and how to measure it. I know that I can't use the part that bows .010" from theoretical straight line at MMC (.124) at assembly.

Thanks

 

[desertfox]

Hi Kinsrow

Any chance of a drawing or sketch?


regards

desertfox

 

[powerhound]

Having a tolerance of +/-.004 with a flatness of .010 on one surface does not make sense, as you stated, because the size tolerance has an indirect flatness control of up to .008 depending on the actual size of the feature. This is consistent with general rule #1. If the actual thickness winds up being .124 then can have no error in flatness. If it winds up being .116 then you can have .008 of error. The .010 flatness is not a refinement of tolerance and thus is illegal.
You may be able to use profile of a surface on the surface that sits flush against whatever it assembles to and unilaterally dispose the tolerance zone to the outside. This will create up to a convex surface when the tolerance zone is used.
Anything I've said really depends on whether I've understood the original question. I'm envisioning a rectangular piece that is 6" long, .25" wide and .124" thick and there may be a counterbored hole on each end. The direction of the bow decides whether it comes out during assembly.

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

 

[dgallup]

It depends on whether you are using ANSI Y14.5 or not. If you are then the flatness must be a refinement of the overall size tolerance & typically less than have the size tolerance. If you are using ISO 8015 then there is no envelope principal and the dimension tolerance is just a 2 point measurement. It can look like a banana for all ISO 8015 cares & you must use GD&T to control form.

In any case you can use a modifier like "NOT CONCAVE" if it is only permissible do deform in one direction.

 

[KENAT]

"ANSI Y14.5" or the current ASME Y14.5M-1994 version. The OP is I believe in the States so I'd guess ASME but it's a good point.

Kinsrow - what standards are you working to as this is a case where it may make a difference.

How about specifiying it in the restrained position and giving the 'clamping' info on the drawing? See section 6.8 of the current ASME standard & fig 6-54.

KENAT,

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

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

 

[TheTick]

The reason the flatness vs. thickness does not make sense is because you're not putting enough thought into it. Thickness is independent of flatness. Imagine a cylindrical tube with the same wall thickness and tolerance. Thickness could be perfectly uniform, in, spec, and the plate still be warped.

Insterad of flatness, try a bilateral profile tolerance.

 

[Kinsrow]

It is per ASME Y14.5M-1994 version. I can't check it when it is clamp because that is exactly what I'm trying to control. If the bow is more than, say, .020" I have to modfity assembly fixture which is a no-no.

I might try Profile tolerance like Tick and Powerhound and see if we have the tools and set up to measure it.

Powerhound,

You understood the part I discribed except I've got many lighting holes between and 2 controlled mounting holes ( one rivet and the other is clearance for screw).

Thanks

 

[powerhound]

Tick,
When interpreting a print to ASME Y14.5M-1994, thickness tolerance and flatness tolerance are related via general rule #1. Saying that the thickness can be uniform but the part can be warped is not correct. If the thickness is at MMC then the part cannot be warped at all nor can there be any flatness error. General rule #1, in a nutshell, states perfect form at MMC. Straightness and flatness are form controls and thus must be perfect if the feature is produced at MMC.
You started out describing a cylindrical tube then finished off talking about a plate so I'm not sure I really understood what you were trying to say. Maybe I'm addressing a non-issue.

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

 

[Kinsrow]

well, I talked to several people including the senior QC and they all said what Tick said. the part can be +/- .004 and can have an additional flatness tolerance of .010". They said that the flatness is reference to it self. This still doesn't make sense to me, but if this is wrong, there are tons of wrong drawings that are released for production. Where exactly can I find this info.

thanks

 

[ctopher]

When I used to design military parts, straightness was the most important. Flatness sometimes, but because of variable tolerances across the surface, they were usually a tighter or looser fit and not acceptable by the customer.

Does this work for you Kinsrow?

http://www.tec-ease.com/tips/july-99.htm

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

 

[KENAT]

"Where exactly can I find this info."

Have you tryed looking in the Dimensioning & Tolerancing standard, ASME Y14.5M-1994?

Specifically 6.4.2. deals with flatness.

6.4.2.1 states:

Where the considered surface is associated with a size dimension, the flatness tolerance must be less than the size tolerance.

I don't know what standard your QC guys are working to but the above sounds pretty definitive to me, unless I'm missing something.


KENAT,

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

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

 

[powerhound]

Kinsrow,

What you describe is sadly an all-too-familiar scenario in the industry that I work in. People running around professing to know GD&T when they have never opened a standard nor have they made the full understanding of it a priority in their discipline. Holding a QM title means nothing in the way of GD&T although it does mean a lot in the world of quality. Likewise, holding a certification in GD&T means nothing in the way of ISO 900* certification but then I never claim to know a thing about it.
General rule #1 is what you're after here. There's no symbol for it so those that think GD&T is all about memorizing symbols don't have a clue that it even exists.

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

 

[drstrole]

Kinsrow, what I believe you are looking for is straightness of a median plane. This would be similar to Figure 6-2 (ASME Y14.5M – 1994, page 158) or Figure 6-3 (page 159), except that the diameter symbol before the straightness tolerance is removed. Note the difference in how it is applied, the straightness tolerance is under the size tolerance, NOT pointing the side view as in figure 6-1 (this is straightness of surface elements. Figures 6-2 and 6-3 allow the boundary of perfect form to be violated. Figure 6-1 does not. Paragraphs 6.4.1.1.2 & 6.4.1.1.3 describe this concept. Hope this helps.

Drstrole

 

[TheTick]

I was't aware of the specific restrictions on flatness and straightness. I was tryng to illustrate how a part can be uniform thickness and still be warped.

If allowable distortion is greater than thickness tolerance at MMC, then flatness would not be appropriate.

 

[ctopher]

Do these help? Sorry they are a bit small. They are as big as I can get them....

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

 

[drstrole]

Ctopher, your bottom example, the straightness of a median plane example, is what I was trying to explain in my earlier post. The shape of the tolerance zone is two parallel planes not two parallel lines, if using Y14.5 definition. See paragraph 6.4.1.1.3 on page 160. This allows the part to bow beyond the boundary of perfect form at MMC.

Drstrole

 

[Kinsrow]

Ok.. If I understand correctly, having flatness call out bigger than the size tol like I mentioned in the first post still doesn't make sense.

Thanks guys.

 

[KENAT]

That's what 14.5 says.

KENAT,

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

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

 

[drstrole]

Don't use a flatness callout, only the straightness.

Drstrole