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

 

[PetkovStoyan]

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?"

The mechanism is actually beater, and at the end of the part there is a beater hammer. During the beating, variable, unevenly distributed lateral forces occur, (in addition to centrifugal forces) which cause the part to rotate towards the adjacent parts. So when a beater hits material, the forces are not distributed only to the two pins, but also on the adjacent "arms" (and their pins respectively), that is if they contact each other. In theory if all four arms are assembled with no gap they will act as a single part, which is more rigid, at least this is my interpretation of the design. Otherwise I don't see why would there be so much small gap, they could've make it larger, 5mm (let's say), which is readily achievable under almost any method of manufacturing, and will not cause headaches to the manufacturer

 

[PetkovStoyan]

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.

Well, I guess a balance between ease of manufacturing, repair/replacement feasibility and operation was intended. All your points are 100% correct.

As for the tolerance scheme, just one question (hope you don't find it dumb) - "datum shift" in simple words mean, that when you place the part on the measuring gage, it is allowed to move within the gap between the gage pins and the holes, is that correct? Since I use MMC, then the pins should be 50,000 mm ***Edit: Actually I think it should be 49,800, since 50mm MMC minus 0.2mm positions tolerance equals 49.8*** (+- some tolerance according to gage tolerance policy), and the part will be allowed to move within the gap between the holes, depending on the exact size of the holes (50 +0,2mm) and the exact dimension between them. Do I understand it correctly?

 

[Burunduk]

PetkovStoyan,
You have the right idea regarding how datum shift works. Regarding the size of the pins that will be used for fixturing: if ⌀50 mm is indeed the MMC of the holes, then your calculation is correct.
Your drawing in the opening post didn't show the tolerance on the ⌀50 mm diameters.
If ⌀50 mm is the minimum limit of size, then ⌀50 mm is the MMC, and your calculated ⌀49.8 mm is correct.
The calculation formula in this case is MMC minus the tolerance of position. It is so because the tolerance of position controls the mutual location between the pins and also encompasses the orientation error that each of them can have relative to datum A. Then the worst case boundary that results takes into account the smallest holes with the biggest inaccuracy relative to each other and to datum A.
This boundary is the size of the fixturing pins, plus and minus a tight tolerance assigned per gages and fixtures requirements. The theoretical boundary is called in the ASME standards MMB - "maximum material boundary", so it is what it sounds like. Because it decides the size of the pins in the fixture, you are always able to fit the part over the inspection fixture. The effect of the datum shift allows the inspector to use the clearance between the actual holes and the inspection pins to move the part slightly relative to the fixture (and as a result, relative to the simulated datum) in case that the measured feature is outside the tolerance zone, and by that to "bring" the feature into the tolerance zone. If this doesn't compromise functional requirements such as some important alignment between components, and if it reflects the way the part is located in the assembly, then it's a good practice that allows fixtures with fixed size elements and less rejected parts.

 

[PetkovStoyan]

Burunduk,

Thank you again for the detailed explanation. The hole diameter limits are 50 and 50,2 so this is the actual calculation.
Thank you for your time and patience.

 

[Burunduk]

PetkovStoyan,
You're welcome.
Just to make sure that another thing is clear:
Datum shift that implies fixed size pins in the fixture is applied when you place the circled M following the datum reference letter in the dedicated compartment of the feature control frame (and then it's called an MMB modifier in ASME). Currently, in your drawing, it is not applied anywhere (you do have the circled M as an MMC modifier, placed next to the tolerance value in a couple of places. It gives bonus tolerance which is different from datum shift, and in your drawing it is only used appropriately with the position tolerance).
If the MMB modifier is not applied, then the default for a hole is that the datum is simulated by a pin with an adjustable diameter that expands until being inscribed by the actual hole (and regardless if the M modifier for the datum feature is used or not, the pin simulating datum B will be very accurately perpendicular to the planar surface that simulates datum A in the fixture). Very likely that you know this already, but I wanted to make sure.

 

[3DDave]

Include the effects of the mating part hole clearance as well.

 

[PetkovStoyan]

Just to make sure that another thing is clear:
Datum shift that implies fixed size pins in the fixture is applied when you place the circled M following the datum reference letter in the dedicated compartment of the feature control frame

Yes, sure, the drawing which I attached to the first post is just my initial attempt, it will be modified accordingly.
I understand from your previous posts that I had to put circled "M" after the datum reference letter, but I didn't understand it completely until your explanation in the las post. Now it makes sense, and I understand what are the real practical implications of that, since until now I just read some theory about with, which didn't make much sense, until you apply it in practice

 

[PetkovStoyan]

3DDave (Aerospace)20 Mar 23 23:33
Include the effects of the mating part hole clearance as well.

Yes, sure, this is important part too. I don't have the drawing of the hub, but I will ask the manufacturer to supply the tolerances of the holes' position relative to the central axis.