How to convert linear dimensions to GD&T

[bc23]

Hi all,

I have 2 dimensions which I hope to change to GD&T control. In the dwg represented below, dim 18 is meant to control the minimum width excluding root radius. Another part will fit in here.
(a) I'm thinking this can be controlled by Profile of surface (with unequal tol). Please advise if there is a better way to control?

(b) Dim 25 is the length/depth of a hole and the intention is to control it excluding the tapered end. A rivet fits here by interference at left side. Can anyone suggest a way to define the FCF?

Thanks
YK

 

[greenimi]

If you can tell us how this part works, what is the design intent mabe we can find a solution together to convert your shown requirements to GD&T
What standard are you using? ASME? ISO?

 

[3DDave]

Feature Control Frames with Geometric Characteristic Symbols control variation limits to surfaces, and do not control theoretical intersections.

You may have to settle for one note to say the full depth of the 2X hole diameter is no less than 24.9 and the full to partial extent of the hole diameter to no more than 25.1 as measured on the mutual axes of the hole from the intersection of the axis with origin surface; use another note to say the dimension as measured parallel to the (axis or bottom surface or inside horizontal surface) shall be no more than 18 and no less than 17.8 to the highest tangency of either radius to the opposing surface.

Alternatively, draw the maximum boundary that the mating part will occupy in the slot and indicate the datum reference frame which should orient and locate the boundary with a note that no material shall be inside this boundary. Add whatever clearance one wants to the volume the boundary controls.

---

Presently there is no such thing as a Geometric Dimension. There are inch dimensions, millimeter dimensions, and so on. I think there are a dozen of types of dimensions; geometric is not one of them, though the Y14.41 committee is dedicated to bringing back the undefined term; advertising teaching services depends on it.

 

[bc23]

If you can tell us how this part works, what is the design intent mabe we can find a solution together to convert your shown requirements to GD&T
What standard are you using? ASME? ISO?

I'm on ISO, but I've found ASME to be quite similar on surface. This part shown is actually a section of a larger part. Basically this part connects to another part which will swivel around the rivet. Dim 18 is important to ensure clearance, dim 25 is to ensure sufficient depth yet not too deep to cause a thin wall on the flange. (& I forgot to mention dimensions are in mm)

 

[bc23]

3DDave
Thanks for the alternative ideas, i'll see how to use it. I've been wondering for some time how to apply FCF to theoretical intersections. There was a similar topic here long ago, but was finally resolved using Position spec.

 

[Burunduk]

Why not establish a datum reference frame from datum features or datum targets and then apply simultaneous profile requirements to the left flat surface and to the right conical end of the hole. Also, a positional tolerance for the interrupted hole in the same DRF. Then do the tolerance stack to see if the distance range requirement is satisfied. It may feel less direct but at least it won't be ambiguous, and will be less risky than any undefined methods.

 

[bc23]

Why not establish a datum reference frame from datum features or datum targets and then apply simultaneous profile requirements to the left flat surface and to the right conical end of the hole. Also, a positional tolerance for the interrupted hole in the same DRF. Then do the tolerance stack to see if the distance range requirement is satisfied. It may feel less direct but at least it won't be ambiguous, and will be less risky than any undefined methods.

Thanks for the suggestion. Profile of surface can be applied to Left flat profile, but for right conical end, I don't know how to measure it. Its difficult for CMM probe to access. Current similar parts are being measured with a combination of gauges & pins (method is easy but has a small stack up error, so I'm trying CMM (& GD&T) to see if I can get more accurate data.

 

[3DDave]

There is always a stack-up error. Using Geometrical Product Specification or a CMM doesn't eliminate this reality of part manufacturing and inspection.

What does the mating pin/rivet do?

If the mating part has a flange, why isn't there a spotface to properly stop it?

If there isn't a flange, what difference does the left-hand face make to the depth when you are trying to maintain a wall thickness on the right?

What spaces the captured part to not move right and left to interfere with the tapered/drafted surfaces?

What do you expect a CMM to measure in terms of where you would have the points taken?

Are those locations different than are being measured now?

What is the exact setup and measuring sequence currently and where does the stack-up error come from?

 

[mfgenggear]

OP
discussion of the length of dim to the drill hole.
the starting point is a theoretical dimension.
that's not the way to design that attribute.
as 3D Dave noted there should be a spot face there. to measure an internal drill hole is a pita. the only way is to make a shop aid locate at start of radius. the included angle can vary for the drill point . which is use to be 118 degrees included. I forget the included angle on the new special carbide drills.
QC, Shop, and engineering must have agreed upon how to inspect a theoretical sharp corner. in this case since it is dimension to a theoretical internal sharp corner is a pita to inspect.
external features can easily be inspected with a CMM and easier with an optical comparator.
so I discourage trying to incorporate profile of any surface. go to the floor and discuss it with a team

 

[bc23]

3DDave, thats a lot of questions, I'll try to clarify:

What does the mating pin/rivet do?
Primarily it allows the mating part (of dim 18) to swivel.

If the mating part has a flange, why isn't there a spotface to properly stop it?
This rivet has a knurled surface at one end for interference fit to the left side hole. Once inserted, it just has to be approximately flush with the left side surface. The "stopper" is from the interference fit and the tapered end.

If there isn't a flange, what difference does the left-hand face make to the depth when you are trying to maintain a wall thickness on the right?
Since the tapered end is also a "stopper", the depth is controlled to ensure the wall thickness on right side is strong enough.

What spaces the captured part to not move right and left to interfere with the tapered/drafted surfaces?
Nothing. Although the part moving in dim 18 has clearance to the draft surfaces, it is allowed to shift left/right (with grease) and basically contact the draft surfaces during movement. There are no functional issues with this.

What do you expect a CMM to measure in terms of where you would have the points taken?
If I create Profile of surface spec's for the pictured part's outer & inner surfaces, I would probe several points on every relevant surface.

Are those locations different than are being measured now?
Yes. Actually nothing is being "measured" now. To check dim 18: the current method uses gauge fixtures & pins to simulate the maximum size of dim 18 mating part. This gives a AC/NC result.
To check depth of pin, a MIN ø pin (longer than dim 25 is inserted and it will protrude from left side hole. This protrusion is judged by a stepped ring fitted onto it, which gives a AC/NC result.

What is the exact setup and measuring sequence currently and where does the stack-up error come from?
Setup & measure sequence as above.
Stack up error for dim 18: the gauge mating part is close fit to the MIN ø pin (error from close fit & from looseness of MIN ø pin); So the mating part is slightly overcompensated for these "errors", and this adds to the errors. (its an indirect checking method based on actual function). I'm wondering is this method common for other industries?
For dim 25: comes from looseness of MIN ø pin.

There are 2 main reasons we want to change the current method:
1. To get data to plot stability of process
2. To have data for troubleshooting purposes
The question of whether these reasons are worth the change was discussed and the consensus was to try first.

Any feedback or comments are welcome.

 

[3DDave]

Nothing indicates that changing how this is specified will change the errors you expect to see.

A picture of the setup is worth 1000 words.

 

[bc23]

OP
discussion of the length of dim to the drill hole.
the starting point is a theoretical dimension.
that's not the way to design that attribute.
as 3D Dave noted there should be a spot face there. to measure an internal drill hole is a pita. the only way is to make a shop aid locate at start of radius. the included angle can vary for the drill point . which is use to be 118 degrees included. I forget the included angle on the new special carbide drills.
QC, Shop, and engineering must have agreed upon how to inspect a theoretical sharp corner. in this case since it is dimension to a theoretical internal sharp corner is a pita to inspect.
external features can easily be inspected with a CMM and easier with an optical comparator.
so I discourage trying to incorporate profile of any surface. go to the floor and discuss it with a team

Thanks for the input.
I've answered about the spot face in my reply to 3D Dave.
I agree that using theoretical dimensions to specify a part is not ideal, so I'm trying to see how i can change it. We have many parts in similar conditions; but because we also design the appropriate gauge fixtures to check theoretical dimensions, there has been no complaint on shopfloor (or QC).
It would be good if I could discuss this w/ QC/shopfloor, however, the sad reality for such matters is they depend more on us (R&D) than vice versa.

 

[bc23]

Nothing indicates that changing how this is specified will change the errors you expect to see.

A picture of the setup is worth 1000 words.

Sorry for my laziness , refer below for measurement setup.

This checks Go & No go (i.e. pin height must be within the step).


This only checks Go.


Stepped ring looks something like this (copied from internet):

 

[3DDave]

Why is the measurement from a surface that doesn't control the depth of the pin?

Since the minimum remaining wall is what is important, then dimension the remaining wall thickness with a stub pin.

 

[mfgenggear]

Thanks for the input.
I've answered about the spot face in my reply to 3D Dave.
I agree that using theoretical dimensions to specify a part is not ideal, so I'm trying to see how i can change it. We have many parts in similar conditions; but because we also design the appropriate gauge fixtures to check theoretical dimensions, there has been no complaint on shopfloor (or QC).
It would be good if I could discuss this w/ QC/shopfloor, however, the sad reality for such matters is they depend more on us (R&D) than vice versa.

Interesting

 

[mfgenggear]

Sorry for my laziness , refer below for measurement setup.

This checks Go & No go (i.e. pin height must be within the step).
View attachment 7314

This only checks Go.
View attachment 7317

Stepped ring looks something like this (copied from internet): View attachment 7316

This the best method. I would suggest to make the drill point optional with flat bottom, using a center cut end mill. then a standard drop indicator with extended tip would be the fastest
Method. Or cmm