Should I include all the details on the parts drawing 4

[Windback]

Hello everyone,

I have designed a steel part for machining and while drafting it, I fully defined all the functional surfaces as precise as needed. Then moved into other features but there are some features that I don't want them to fully dimension and restrict with tolerances because these features would be ok either way. The reason is that I don't want to deal with non-conforming parts at the end...

On the other side, ASME Y14.5 PARA 1.4b states "Dimensioning and tolerancing shall be complete so there is full understanding of the characteristics of each feature.". I got confused here, what should I do should I follow the standard or should I stick into engineering intent? What is the general practice for these situations. Any comment, advise and/or idea will be appreciated.

Thanks in advance.

 

[JohnRBaker]

What sort of "features" are we talking about? Blends/Rounds, Chamfers/Bevels, ??? And if you're not concerned about their dimensions or tolerance, then what purpose do they serve?

John R. Baker, P.E. (ret)
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[BrianPetersen]

Unless you have a good knowledge of how the part in question is to be manufactured (in which case, you wouldn't be asking the question that you asked ...) Step 1 is to have an in-person discussion with whoever you propose to manufacture the part in question, to see what information THEY need, and to incorporate any ideas that they have to make manufacturing the part easier.

Step 2 is to refine the part and its dimensions and drawings to include your new-found knowledge, with intentionally loose tolerances applied to the dimensions and features that you are not all that concerned with.

 

[rb1957]

you can dimension them as "reference" if you don't want to call out a specific dimension.

else you can give a very sloppy tolerance, and for your piece of mind remodel with the extreme tolerances (this is something you keep on the side in case there is an issue later, and people start blaming you).

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[mfgenggear]

windback
it is bad practice when inspectors and machinist have to guess what an engineering drawing requires because of lack of information.
if it not important on the drawing then it specify on the drawing.

 

[Jboggs]

I like the "REF" option. I use it not to define the part, but to assist the user in understanding what he's dealing with. In my mind any dimension marked "REF" should not even be checked by an inspector for the purpose of accepting or rejecting a part. It is there only as a courtesy to the user from the designer.

 

[drawoh]

Windback,

Every single feature on your part must be dimensioned and toleranced.

People now use model based definition (MBD). Dimensions are extracted from the 3D[ ]STEP file you attach to your purchase order. You have a note on the drawing specifying the profile and other tolerances of features not explicitly dimensioned.

--
JHG

 

[SnTMan]

there are some features that I don't want them to fully dimension and restrict with tolerances because these features would be ok either way

Hard to know what this means exactly.

Reference dimensions per Jboggs are often useful...

Regards,

Mike

The problem with sloppy work is that the supply FAR EXCEEDS the demand

 

[TheTick]

I see a lot of blanket surface profile tolerances on molded parts. This covers anything not explicitly dimensioned.

Usually I see surface profile of some value relative to three datums, but I believe less is more in this case. Over-constraining the blanket profile tolerance can have unintended consequences.

 

[rb1957]

our drwgs have standard tolerance ... 1 decimal place means 0.1" tolerance, 2 places 0.03", 3 places 0.01".

yes, many machined parts made to models (STP files). The problem is what do Inspection use to check the part, so we have to issue drwgs with a few dimensions and a note "refer to CAD model for missing dimensions".

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[drawoh]

rb1957,

I have set up drawing templates here with a note stating that undimensioned features have a profile tolerance of 0.8mm. Any reference dimensions I throw on are controlled by that note. The old note that specified tolerances by the number is decimal places, is not compatible with ASME[ ]Y14.5, which requires that trailing zeros be removed from metric drawings.

--
JHG

 

[rb1957]

ok, our practice is like JBoggs above ... "any dimension marked "REF" should not even be checked by an inspector for the purpose of accepting or rejecting a part. It is there only as a courtesy to the user from the designer."

one example is redundant dimensions, where in a view it helps understand the design to have a dimension that is actually defined by other dimensions in other views.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[CWB1]

Yes, prints should be fully detailed. Most dimensions shouldn't have a tolerance callout explicitly attached, they should be basic dimensions implicitly governed by standard/"title-block" tolerance and GD&T. Your standard tols/GD&T should be loose for the specific manufacturing process so easily/quickly applied.

Reference dims tend to cause trouble bc they're commonly over and incorrectly used, so I'd limit or avoid their use entirely. Used properly they provide no info that cannot be calculated from the print, they simply save the calculation but can be rather misleading when tolerancing is applied, thus cannot be used for inspection or anything critical.

People now use model based definition (MBD). Dimensions are extracted from the 3D STEP file you attach to your purchase order. You have a note on the drawing specifying the profile and other tolerances of features not explicitly dimensioned.

MBD doesnt use a print, it uses notes, dims, and GD&T embedded into an additional layer of the model itself to communicate with inspectors. Most of industry has chosen not to adopt its use bc there are many folks in purchasing/manufacturing/etc that need access to data but simply dont have modeling experience; the various modelers also tend not to talk nicely with embedded notes. I worked at one of the few companies that successfully adopted it, but they had very little outsourced manufacturing.

Providing suppliers with both 3d & 2d is good and standard practice, but the word of caution I always add is to be careful with the master/slave relationship. In western countries the 3d model is the master data whereas in Asia/east the 2d print is master.

 

[drawoh]

CWB1,

I am having problems with this concept of master and slave applied to drawings and models. Any dimensions and tolerances called up on the drawing must be met. My drawing has a note stating that any features not dimensioned are controlled by the 3D[ ]STEP file. I have learned that the STEP file must be modelled to median condition, i.e., half way between the MMC and LMC. Any reference dimensions I apply to the drawing actually are inspectable, because I can verify that they comply with the general profile tolerance specified in my notes.

Master and slave have no meaning unless the drawing and the 3D[ ]model differ. If they differ, I would strongly prefer that the fabricator contacted me and ask for a resolution. There are no acceptable explanation for this situation.

--
JHG

 

[Orange_kun]

If you don't care about the feature, why is it even on the part? Workholding? Then have a note saying so, and list the acceptable MMC/LMC.

My company always supplies a drawing, a step file, and an x_t file for manufacture. The model is supplied at nominal size. Where possible, I like to use symmetric tolerances, but if the application is a shaft/hole fit... use those and force the fabricator to employ tool path offsets.

A blanket profile tolerance is super helpful for keeping drawing simplicity. For my small parts, I'm often saying a profile tolerance of 1mm is acceptable unless otherwise specified. If I have a tricky surface I need, the model shows the details and I just put a tighter surface profile on it, and TALK to the fabricator. Particularly if there is a unilateral callout... communication is key.

But if you have features that really don't matter, you should still put a boundary on them. Otherwise you really need to think hard about what happens if the feature is missing entirely, or 2x as big. Is that acceptable? Or not really? Tolerance everything.

 

[Windback]

First of all, thanks again to everyone that helped me while figuring out the issue I had. I've talked with my supplier and just put a REF dimension for that feature. So I'm ok now.

There are a simple questions I ask myself when I start a drawing:
What do I need?
What do I want?
If I can't answer those questions, then the person reading the drawing can't either.

Hold on, this is not an answer for the question. Here nobody asks you how to design/dimension a part. The question is about a specific case.

If you don't care about the feature, why is it even on the part? Workholding? Then have a note saying so, and list the acceptable MMC/LMC.
My company always supplies a drawing, a step file, and an x_t file for manufacture. The model is supplied at nominal size. Where possible, I like to use symmetric tolerances, but if the application is a shaft/hole fit... use those and force the fabricator to employ tool path offsets.

I didn't say I don't care about "the feature" I think I was saying I don't care only 1 dimension of the feature I care the other 2 dimensions... I think I was said don't wanna "FULLY" dimension a feature.

Hard to know what this means exactly.

I think a lot of professionals here got understood what that means. If you be specific about the point you cannot get I can help you.

 

[3DDave]

I would like to see an example of such a feature as depicted on a drawing.

 

[3DDave]

Here's an earlier discussion on the opposite problem:

https://www.eng-tips.com/viewthread.cfm?qid=322065

Also

https://www.reddit.com/r/engineering/comments/g65wfr/how_many_critical_dimensions_is_too_many/

Not good results for:

https://www.google.com/search?q=only+putting+important+dimensions+on+drawings

https://www.google.com/search?q=leaving+off+unimportant+dimensions+on+drawings

There is the concept of the partial dimensioned drawing - but that always requires a solid model to go along with it from which the feature dimensions are extracted.

If you are worried that a huge tolerance zone on a feature might lead to rejecting a part, I'd worry that none of the other tolerances will be met.

 

[Jboggs]

"I would like to see an example of such a feature as depicted on a drawing."

Consider an assembly drawing of a mechanism. It would be helpful to the folks that will have to deal with that assembled mechanism (lift it, pack it, move it, whatever) if they could have some idea of the overall size, or weight, or CG location, or the location any particularly sensitive areas, etc. So, for those and similar purposes the designer might include that information on the assembly drawing. That information is not there to define the part. Its there to give those that have to interface with the part some idea what they're dealing with, thus the "REF" callout.

 

[3DDave]

Jboggs - it's a steel part, not an assembly, and it's for the manufacture of said part and all its features.