GD&T of extruded part with irregular profile 1

[PetkovStoyan]

Hello,

I don't have experience with GD&T, but I wanted to use it on a particular part. I read some materials on the fundamentals of GD&T, but unfortunately all examples were fairly simple parts with straight prismatic surfaces. My part has fairly irregular profile, meaning it has no straight surfaces to use as datums (except the top and bottom, since it is extruded part). I have attached sketch of the assembly and the part in the area concerned. (I also attached an image, since I'm not sure the .pdf file uploaded successfully) Four parts are attached to a hub with the help of the two holes 50mm dia. and pins. The gap between two adjacent parts is 0,7mm, and the gap between the part and the hub radially is 3 mm. I want to add geometric tolerances in such way, that there is minimal gap guaranteed. For example 0,7mm gap to be at least 0,3mm (let's say) in the worst case, and the 3mm gap to be 1mm in the worst case. Since the values are different, I will have to use separate tolerances, rather than single profile tolerance, otherwise the precision will be increased unnecessarily in the area of R105,5 segment.
Not sure how to do this properly, I have provided some possible (maybe wrong) solution. Please help me to do this correctly on the drawing.
The values provided are just for example, I will have to do some calculation to determine the exact values, any help will also be appreciated on this too.
The idea is to use the bottom as first datum, and both holes as secondary datum, which are drilled reasonably accurate possible for this type of heavy part

My main concerns are:
1. Is it good practice to provide basic dimension from non-existing entity, particularly dimension 157,1mm from center of circle?
2. What is the best practice to position the inclined 45 deg. surfaces, is dimension 64,7mm adequate?
3. Should I use angularity tolerance or profile tolerance for the two 45 deg. inclined surfaces?

https://files.engineering.com/getfi...-4865-b649-e450b7937d24&file=GD_T_Example.pdf

https://res.cloudinary.com/engineering-com/image/upload/v1679089179/tips/GD_T_Example_e1qnix.jpg

 

[Garland23]

For having no experience with GD&T, that's not a bad attempt!
One of your questions was about datums from irregular shapes; there is a special way to do that called "datum targets." But I think your datums are OK on this one.
The difference between angularity and profile of a surface is that profile of a surface has the additional power to control location. If you go with that, then the 64.7 dimensions would not have plus/minus; they would be basic. Therefore, it comes down to what the function requires. If you do keep angularity, though, you'd have to drop the "M" modifiers because those only get applied to "feature of size" GD&T callouts.

 

[3DDave]

" I will have to use separate tolerances, rather than single profile tolerance, otherwise the precision will be increased unnecessarily in the area of R105,5 segment."

You can specify any profile of surface tolerance you like, and as many as you like, to have whatever precision you like over whatever range is required. You can even make it with an offset so that the limit of material is one boundary of the profile zone to make such calculations easier.

More datum features are unlikely to help this case unless you have surfaces that are forced into contact, as datum feature A is.

 

[PetkovStoyan]

Thank you both for your replies.

Any guidance on how to calculate the exact values?

 

[3DDave]

Not yet - since the pins are what precisely locates the part in the assembly why do you care so much about the gaps?

Also, you have no information about the portion that trails off into thin air. Is that important and can the pins be really loose and let the other parts just rattle about?

 

[PetkovStoyan]

"since the pins are what precisely locates the part in the assembly why do you care so much about the gaps?"

Because if any gap disappears due to poor manufacturing, and the parts collide, even if the holes' locations are perfect, it would be impossible to insert the pins thru all parts, since the part will be offset due to the collision. This will happen if, for example, dimension 64,7 becomes 65,7 in the real part, since 1mm more will eliminate 0,7mm gap. The same will happen if 45 deg. dimension deviates, or combination of both linear and angular dimension deviate to some extent, which is inevitable. This is the general idea - to limit these deviations in such way, so that some gap is guaranteed. Otherwise the adjacent parts will collide, and very likely the assembly becomes impossible.

I wouldn't say that the pins are loose, rather there is minimal gap between them and the other parts. Due to difference of hole location between the hub and the part in interest, the pins almost certainly will touch the holes in minimal surface, close to line. This is inevitable, since the part and the hub are not manufactured as a set, and hence the holes are not machined together, there will be always some off-center distance, depending on the precision of the machine. I made and attached exaggerated sketch to illustrate what I mean, I've shown the extreme case where one of the dimension is equal to its upper limit of tolerance, and the other is equal to its lower limit of tolerance. The pins are manufactured with negative tolerance, in order to accommodate this, precisely, the pins diameter is 49,8mm. We have tried before with more precise pins, I think it was 50h6, or something like that, but we had problems with extracting them during the replacement of the parts, they tended to seize a lot. This is also a factor to consider. But in general you are correct - there is a possibility to have gap between the pins and the other parts assembled. The pins are not press fitted, and are secured against self-extraction via other means.

As far as what lies beyond the cut-off of the view, it is not much of importance, there is a lot of space, and large tolerances. The problems we have are where all parts assemble to the hub. If you insist I can show it anyway.

https://files.engineering.com/getfi...-1997c751bec4&file=2023-01-20_Biela-Model.pdf

 

[PetkovStoyan]

"One of your questions was about datums from irregular shapes; there is a special way to do that called "datum targets.""

Garland23,

after thinkin a bit more on this subject, I think my confusion comes from the fact that I think for manufacturing and inspection in the same time. In order to comply with dimension 157,1, you have to find where exactly is the center of the surface C-D (R105,5), and I think therefore you have to use it as datum before drilling the holes, that is if the outer contour is manufactured on separate machine, for example plasma, or water-jet cutter .
But that will not be necessary if you inspect the part. In general all GD&T on the drawing is related ONLY to the inspection of the completed part, this is correct, right? It is not related to any intermediate operations, right?

 

[Garland23]

It's better to always emphasize the function when designing parts, instead of focusing on manufacturing or inspection. There are exceptions to this idea, but it's a general rule that usually helps everybody in the long run.
To your specific question, the profile tolerance is centered around the R105.5, which itself is located from the 157.1. However, the profile tolerance already mentions datums A and B, so the center of the two holes is really what locks in that profile tolerance (if you chain together the 157.1 and the 105.5).
So don't worry about making a datum from the curved surface -- it's already driven by where the two holes are (datum B).

Edit... If you think that the function mandates that the curve be the driving factor (rather than the holes), then you could create a datum down there, and then position the holes to datums A and the new datum B. But you'd need a third datum also, to constrain the rotation.

 

[PetkovStoyan]

If you think that the function mandates that the curve be the driving factor (rather than the holes), then you could create a datum down there, and then position the holes to datums A and the new datum B. But you'd need a third datum also, to constrain the rotation.

Actually this describes exactly my problem. The holes shall be the driving geometry since they position and orient the part, they are the functional entities. The curve has to follow in order to guarantee some minimal gap where appropriate, it is not functional, just have to ensure gap in certain limits.

The actual problem is that the manufacturing process is the other way around - first the curve is created with less expensive process in order to reduce (or eliminate at all) machining time - plasma, water jet, laser etc., and after that the holes are created. The critical surfaces then can be machined if necessary. And that's why I am running in circles of self-dependency of the entities, and cannot wrap my head around it.
So in reality the part should be positioned the way you describe it at the end of your post, before drilling the holes. The toleranced surfaces must be checked for compliance, and machined if necessary. So a sort of combined measuring/machining custom jig will be needed.

 

[Belanger]

The holes shall be the driving geometry since they position and orient the part, they are the functional entities.

Then what you originally have is indeed correct. As Garland23 mentions, it's the function that matters. We (and you, if you're the designer) shouldn't care how the part is made. For all we know, they could throw the part up in the air and shoot some bullets in order to make the two holes
By following the function-first philosophy, it actually liberates the manufacturing folks to make the part using whatever sequence they think is best, as long as the final dimensions and tolerances will pass.
So if the holes are what align the thing in its assembly, then keep them as datum feature B.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[PetkovStoyan]

We (and you, if you're the designer) shouldn't care how the part is made. For all we know, they could throw the part up in the air and shoot some bullets in order to make the two holes

Well, in general you are right. But if you happen to work in enterprise where you have both design and manufacturing dept., then it is sure that the designer shall be asked to come down to the workshop to explain how exactly to make the part.
I always try to "step into the shoes" of the manufacturer, because sometimes it may happen that you require impossible or impractical things. It's always good to check yourself

 

[3DDave]

There is a fundamental difficulty posed in the problem statement. Most often parts are designed with the requirement that the parts can be positioned such that all features involved find a single mutually satisfactory position. While there may be more than one, only one is required.

Your application is to ensure that the clearances are guaranteed over every possible location and orientation from every possible variation.

This is normally managed by interference fits, to ensure there is only one possible location and orientation for any particular assembly, but the clearance fit with the pins means a larger range of motion, including translation and rotation and those affect the clearance(s) of interest. These effects aren't controlled directly by geometric tolerance characteristics, assuming controlling them that way is the goal.

This will be made worse to analyze if the holes in the clevis are allowed additional clearance. Since there's a group of holes in the clevis the clearances of interest is also influenced by the locations of those holes relative to one another.

edit: fixed minor typo.

 

[PetkovStoyan]

3DDave,

You are 100% right, this is fundamental problem of the part, but I don't know how can this problem be solved, since the part and the hub are not manufactured simultaneously, because the part wears fairly quickly, and we replace them rather often. In theory one possible solution is to use interference fit at one of the holes, and use the other just to constrain rotation. But in reality the design was created long ago, the equipment is operational, and this would mean rework of all hubs, which will be practically impossible. So I am stuck with this inherent problem, and I just want to try to solve it the best possible practically way.

Is there a way to take all factors into consideration when calculating the side gaps, including holes and clevis tolerances? Maybe with the help of software, I have Inventor 2015, is it capable of such calculations? I know SolidWorks has DimExpert for such calculations, but again I am not sure if it will be capable in this particular case

Edit: I've found one video on youtube, which describes this problem in detail. The displacement between the parts is called "Assembly shift", I don't know if this is the conventional name, and it is explained how to calculate it.

https://www.youtube.com/watch?v=qAsE3L3ChmM.

Maybe I can calculate this, and then use to value to calculate the geometry tolerance values that I need.
I've also tried TolAnalyst study in SolidWorks, and checked the checkbox "float fasteners and pins", but I cannot understand why the pin tolerance is not listed in the contributors box. One would think that if pins are really floating, their tolerance will contribute to the overall deviation.
What mates should I use in the assembly of the pins with the other parts - concentric? It is little counterintuitive, since in reality the pins will not be concentric almost all of the time

 

[Burunduk]

The clearances between the holes and the pins can actually help you to adjust the gap - move the parts slightly to create the gap when the parts are touching. If you want to ensure that the parts are not interfering at the worst case you simply assume the part is fixtured by the base face and the holes without ability to move at all, as if it was an interference fit, and then determine the boundaries that would prevent a zero gap or a gap that is too large, and control the relevant surfaces by profile of a surface relative to your current A,B DRF. You also have to take the mating part's tolerances into account (the pairs of holes can be drilled closer or farther away from each other).

Don't keep the 64.7 distances from the hole centers to the edges directly toleranced because such a requirement is ambiguous. It's not defined how the centers of the holes are established, and the tolerance zone is not robust.

Back to the topic of the "play" which is possible due to the clearance fit at the holes - if by chance you are working according to the ASME Y14.5 standard, you could actually take advantage of it to allow additional variation for manufacturing as "datum shift", by adding the MMB modifier following the datum reference later B in the feature control frame (tolerance frame). But I have a feeling that you are not following the ASME standard, may be ISO where this is not available if I'm not mistaken. Is that correct?

Edit: it seems like the circled M modifier on the datum reference is also available in ISO-GPS, and it's called "MMVC" or "MMVS" (both correct?) so you can probably implement this to give manufacturing more allowance for variation.

 

[PetkovStoyan]

Back to the topic of the "play" which is possible due to the clearance fit at the holes - if by chance you are working according to the ASME Y14.5 standard, you could actually take advantage of it to allow additional variation for manufacturing as "datum shift", by adding the MMB modifier following the datum reference later B in the feature control frame (tolerance frame). But I have a feeling that you are not following the ASME standard, may be ISO where this is not available if I'm not mistaken. Is that correct?

To be honest, I am not following any standard, but I presume ISO shall be applicable, since we are in Europe.
I wrote in the beginning, that I have no prior experience with GD&T, I just wanted to improve the existing drawing, since the tolerances in it are not adequate, there are no geometric tolerances, just linear symmetric tolerances. I read some fundamental theory on the subject, but little did I know that this part will be such a nightmare to tolerance properly, and apparently more advanced knowledge is needed, and experience of course.

 

[Burunduk]

You are on the right track to improving that drawing. I second what Garland23 said:
"For having no experience with GD&T, that's not a bad attempt!".

Just fine-tune it according to the tips you were given so far:
Get rid of 64.7±0.2 and replace it with a basic (theoretically exact) dimension. Consider replacing the angularity tolerance with a profile tolerance that can control location of surfaces in addition to the orientation (it can perform the function of 64.7±0.2 much better, and control the angle at the same time). If it is from some reason important to maintain a tighter angular control on the 45° than the control of location, keep the angularity tolerance as a refinement of profile (the angularity will be required within a tighter value than profile). Don't use the MMC modifier on the tolerance value for a planar surface. It is applicable only to features of size (for certain types of geometric tolerances - angularity included, but again, only for features of size).
Consider "datum shift" applied through circled M following the datum reference B letter in the feature control frame once you apply profile of a surface, and for angularity - if kept as a refinement. It will relax the requirements while not compromising the functional need to prevent the parts from interfering with each other (taking advantage of the play between the pins and holes due to clearance).
Once you applied the geometric tolerances, simply model your parts at the worst case limits and see how they assemble. Adjust the tolerances if needed and make sure you are ready to explain the meanings of the renewed drawing to the manufacturing department - work in close coordination with them so that they are not surprised when they receive the revised drawing to their desk.

 

[3DDave]

PetkovStoyan,

The first step is to decide what will restrain the part and how much assembly shift will be allowed. Then apply the hard limits with those shifts as if those limits were grinders or saws to remove material. The overall combination of all movements of the boundaries relative to the accepted restraints will remove all non-compliant material.

This will form the exact profile that is the maximum outline.

I presume in Solidworks you can assemble multiple copies of a part that is initially represented by a plate with holes to as many limits as you like and then use then use the desired limit to create cuts in the assembly using the limits you like to each of those copies? Reduce the diameter of the simulated pins by the diametral location and clearance of the pins in the hub holes.

Apply a one-sided profile tolerance to that border by using a curve to represent whatever clearance you want and then see that the conditions you set are always met.

 

[PetkovStoyan]

I think I will reconsider the tolerance scheme, I think I have got it wrong all along.
This part is classic case of floating fasteners assembly. Meaning, that when you position the part in such way, that the 0,7mm gap is present, it should be possible to insert the pins, i.e. it should be possible to be assembled. Then if some play of the part occurs due to hole/clevis tolerances, OK, no harm, the worst that could happen is that two adjacent parts will touch each other, the important is that the assembly was possible. I think that this is even desirable, so that the forces during rotation are not solely absorbed by the clevis, but the adjacent part also supports and absorbs some of the forces, maybe this was designers' intent. And maybe this happens after some working time, since I've seen deformed holes on the parts.

In such case the two inclined 45 deg surfaces should be the second and third datums, and the holes should be aligned according to these datums.

 

[3DDave]

Rotation usually sends parts away from the axis of rotation and from other parts also tied to that rotation. Is this hub not the rotation center? And how does adding forces from one part onto another part that already has loads cause those loads to be "absorbed?"

 

[Burunduk]

If the parts are only located by the holes and they are not clamped in place in any way after assembly then the exact gap distance is anyway uncontrolled and will not be constant. The parts will rattle as the assembly starts to rotate until stabilized by the centrifugal force. I don't know if this is acceptable and it is surely unusual for a rotating mechanism. I think it is not ideal for most applications to say the least, but if it has worked that way so far for years and everyone is happy and you say it is not your goal to redesign the fit - I suppose that's OK. If you only want to improve the drawing and mainly make sure everything fits together, then as it was suggested, profile tolerancing to control the variation within the required limits with reference to the A(planar surface), B(holes) DRF is fine.