Assembly level dimensioning 1

[AMontembeault]

Having a bit of a philosophical debate at work, and I was curious what a broader community might think.

ASME Y14.5-2018 Section 4.1 (p) states "Dimensions and tolerances apply only at the drawing level where they are specified. A dimension specified for a given feature on one level of drawing (e.g.,a detail drawing) is not mandatory for that feature at any other level (e.g., an assembly drawing)".

So suppose we have a piece part with a feature or group of features which are appropriately toleranced and controlled at the piece part level - let's say it's a hole pattern. Now let's say that the same pattern is used to help establish a datum reference frame at an assembly level. The question then becomes if it is right to dimension and tolerance these features again at the assembly level, given the requirements of the previously mentioned section 4.1 and additionally the requirements of section 7.5, or if it is appropriate to call these features out by reference dimensions, since they are already established in the real world? Or perhaps its unnecessary to call out the size tolerance of the holes, but necessary to call out the datum controls to higher precedent datums?

On one hand, "letter of the law" seems to indicate that its necessary to call out all dimensions and tolerances again, even if they're the same as what was previously on the piece part drawing, in order to establish the true geometric counterparts at the assembly level. On the other hand, it seems inefficient to require additional inspection of features which were already inspected and unlikely to change due to the assembly process.

My personal feeling is that we probably should call out the dimensions and tolerances again. There's no guarantee that the supplier producing the piece part is the same supplier producing the assembly, or that either supplier is producing fixtures for said assembly or inspection of the assembly, which means piece part drawings would have to be supplied in addition to assembly drawings to all suppliers.

Curious what others think...

 

[jassco]

Hi, AMontembeault:

The physically same holes on your assembly are different from those on components. Sizes and position of the holes on the assembly are specifications for the assembly while position and size of the same holes on the component are specifications for the component. Both set of holes are evaluated separately because they belong to two different items. The issue is what you are going to do if those position and size on the assembly do not meet their specifications. Are you going to "perform" an assembly operation to bring them into specification?

Best regards,

Alex

 

[drawoh]

AMontembeault,

I subcontract fabrication of 123-456 MACHINE BASE, and I use features of this as datums on assembly 123-771 THINGAMABOOBER. The assembly drawing has dimensions and tolerances, because stuff has to be adjusted.

Billy Bob and Cousin Elmo's machine shop fabricates the machine base as per my drawings, which show the dimensions and tolerances of all the features, including the critical datum ones. Everything is called up as per ASME Y14.5-2018. We inspect the parts at our loading dock.

My assembly drawing shows the dimensions and tolerances of the datum features as reference dimensions, perhaps complete with tolerances. The assembly people have no control over these dimensions and tolerances, but the information is potentially useful. The assembly drawing will have dimensions and tolerances on it as per ASME Y14.5-2018.

The datum features are fabricated by Billy Bob and Cousin Elmo. The assembly team has no control over them, however concerned they are. The optical alignment on the thingamaboober will be insepcted.

The real, toleranced dimensions go on the drawing that will be used for fabrication/assembly, and inspection. They may be added as references on other drawings.

--
JHG

 

[3DDave]

Not repeating them as firm dimensions and tolerances means they cannot be used to establish a DRF at the assembly level. Reference = safely ignored. While the features themselves are not controlled by the assembler, any virtual condition that may apply at the assembly level with regards to their use as a datum feature definitely does affect acceptance at the assembly level.

 

[pmarc]

I agree with drawoh.

While exceptions may happen, I believe the assembly supplier should not generally be held acccountable for the conformity of already existing features to the requirements defined at the lower-level drawing(s). If virtual conditions for these features affect acceptance at the assembly level, the assembly drawing should contain all necessary information allowing to calculate the virtual conditions properly as reference information for the assembly supplier.

One way to address this problem (at least partially) is to specify the virtual condition sizes directly in the FCFs, as shown in para. 7.11.10 in Y14.5-2018, on the assembly drawing.

 

[3DDave]

So, copy and display all the same dimensions, same references, and then add an additional calculation? More steps = more errors. It can work but is not necessary.

It seems like the purpose of explicit Virtual Condition values was to reserve mobility that the usual calculation would give up rather than as a work-around to putting "do not alter item features to meet requirements" on the assembly drawing.

The underlying concept remains - the assembler is never required to get the part drawings to find out what the lower level requirements were and should have that information on the assembly drawing.

 

[Burunduk]

This corresponds with another problem:
There is "(p) Dimensions and tolerances apply only at the drawing level where they are specified", and there is also "(a) Each feature shall be toleranced".
So if tolerances on the detail drawing do not apply at the assembly level, doesn't it mean that any features left without tolerance specifications on the assembly drawing (because their tolerances are already covered in the detail drawing) are essentially considered untoleranced for the assembly level? Doesn't it make the assembly drawing non-compliant with the Y14.5 standard for not satisfying fundamental rule (a)?

 

[3DDave]

That oversight is due to the close participation of inspectors, inspection software makers, and sellers of training to support piece part definition to the detriment of looking at how the final system is to function. As long as one looks at the problem through the soda straw of getting parts through QC then one gets large gaps.

 

[jassco]

Hi,

Let's say you have two arc segments that need to be welded. You need to specify a radius for the arc on component level. But you will also need to specify a radius on assembly level so that when they are assembled or welded, the radius on the assembly is not out of specification.

The radius on the assembly print is different from that on the component print even though they may be same or equal.

Best regards,

Alex

 

[ASIT859]

I've just recently needed to deal with something like this. It's currently unproven since we haven't produced yet, but I've gone with the following method following a description of the process since I think specifics might help.

- My product is a casting, but some of the datum target locations we use to inspect the casting are removed during machining process OP2. We had a very difficult time avoiding this, so we came up with the following.
- For machining process OP1, we have a dedicated drawing and this machining step produces the datum features for OP2. We did this to allow traceability from OP1 back to casting, and from OP2 back to OP1, but not OP2 back to the casting. This is why we went with separate drawings.

The OP1 drawing uses the casting DRF and specifies 2X holes. Those are defined appropriately with basic dimensions for position, sizes directly toleranced, and a position callout as well. The position is specified at MMC.

The OP2 drawing calls out each of the two previously machined holes and has their nominal size and size tolerance specified in parentheses. The holes are positioned with reference dimensions to one another. New features are then dimensioned accordingly from these holes. What I don't have included is a feature control frame specifying the positional tolerances between holes to give the inspectors enough information to know the true geometric counterpart. The original idea was for them to have access to the OP1 drawing.

I think what I'll do is for any feature control frame referencing these hole datums, is to explicitly specify the datum boundary IAW the 7.11.10 paragraph in Y14.5-2018.
I'm also now not sure if the location holes on the OP2 drawing should remain as reference (since they were completed in OP1) or if I should make them basic.

I hope my description makes sense and is helpful for the discussion.

 

[3DDave]

They should be basic.

On the topic of reference dimensions: "It is considered auxiliary information and does not govern production or inspection operations"

 

[Burunduk]

ASIT859,
Does the OP2 drawing describe the final product?
Are the holes produced in OP1 used as a primary reference for the DRF of the OP2 drawing? Or maybe secondary, or tertiary?

In general, in a final product drawing, the datum feature selection and their precedence in a DRF, as well as their tolerancing, should be functionality-based, not process-based.
If, for example, the pair of holes is used as a primary datum reference (constraining 5 degrees of freedom unless they are coaxial, and then it's 4), their size should be toleranced in the same (final) drawing and their mutual location should be controlled by a position tolerance. No reference to any previously (or currently) existing features used as manufacturing references is required - those can be applied in the process drawings like OP1 and the casting. And if the size was already inspected at OP1, it doesn't mean it shouldn't be specified on the OP2 drawing. It only means that this particular tolerance is inspected "in process", which is fine. The way I see it is this - if OP2 is final, the OP1 drawing should have matching tolerances to OP2. The final drawing drives the requirements for all the preceding manufacturing steps, not the other way around.

 

[ASIT859]

@3DDave, thanks - I now agree that the hole to hole spacing should be made basic.

@Burunduk,

The OP2 drawing does describe the final product.
The holes produced in OP1 are the primary and secondary references in the OP2 DRF. The tertiary is actually the milled face that the holes are machined into. The holes are functional as they are dowel holes used to mount a manifold to the product.

The main DRF on the subject item is made of the first dowel hole (4-DOF), the second dowel hole (1-DOF), and then finally the plane (1-DOF).

I like your suggestion and it does indeed make sense to me. I suppose there's really no harm with specifying the two dowel holes with size tolerances and positional tolerances on the OP2 drawing (in fact it may be the correct method) - it's not like the OP2 machinist will see the drawing, see the part, and then run the machine to reproduce those holes when they're already there. As you say, they can simply check those holes in-process and move on to the rest of the machining. I hope my understanding of your comment is correct.

Back to the main topic and subject line of this thread - while my particular product is stages of a single item (casting), we do currently produce an equivalent product that is a welded assembly made of five separate parts. The series of individual component detail drawings, welding drawing, and final machining drawings follow the sort of flow that I've described above. The current project I'm working on is to replace this costly weldment with a lower cost casting due to the reduced handling and labor.

 

[Burunduk]

As you say, they can simply check those holes in-process and move on to the rest of the machining. I hope my understanding of your comment is correct.

Yes it is.

The series of individual component detail drawings, welding drawing, and final machining drawings follow the sort of flow that I've described above.

I believe that the same principle applies. The final drawing that describes the finished part after the castings, intermediate machining operations, welding, and final machining, should be fully defined with all the functionally appropriate tolerances - of both datum features and features that are controlled relative to them. The in-process drawings that describe the components and their different manufacturing steps should also be fully defined, and features that will remain unchanged in the final part should have tolerances that correspond (tighter or at least equal) to the finished part tolerances. In short, the In-process drawings should be toleranced in a way that will allow the finished part to meet the final drawing requirements.
The machinist that will work to the final product drawing will have only the features he produces and has to inspect marked up on his copy of the drawing.

I think that with welded assembly drawings things are relatively easy and the rules of ASME Y14.5 make sense. I have much more trouble in understanding how the same rules (those I mentioned in my 20 Sep 23 20:45 post) apply to separable assemblies of rigid parts, in which the geometry of the components is not altered in the assembly process. I'd be happy if someone elaborated on this.

 

[Eric Gushiken]

Hi AMontembeault,

Just curious. How tight is the positional tolerance for the hole pattern? If there is a certain tolerance requirement at the assembly level for these holes I believe the positional tolerance at the part level would need to be tighter because of assembly tolerances. You'd need to do a tolerance stackup to determine how tight the assembly level positional tolerance needs to be. Also, you mentioned that one of the hole patterns is being used as a datum feature at the assembly level. I think this would mean that those holes would be indicated at MMC which may give you some datum shift and allow you to help meet the tolerance on the other set of patterned holes.