Tolerances on Mech Drawings 9

[Metalguy]

Many years ago when I took a HS course in mech. drawing, the correct way to show dimensional tolerances was to have the same number for the + and - eg., if you want something between 7 and 9 in. long you used 8+/- 1 (I can't figure out how to get the + directly above the - here).

But the foreign co. (Italian) I'm working at has a weird (to me) way of showing them. They'll use anything from 7 +2/-0 to 9 +0/-2. They've even used (I am NOT making this up!) something like 6 +1/+3!!! This is not a small company, but a fairly large but old manufacturer of BIG equipment.

Anyone seen anything like this before?

 

[ctopher]

All CAD models should be created at the mean dimension, or nominal/middle. However you read it. For reasons to use on CAM, FEA, CAE, DXF, and most major companies prefer it for mockup use.

http://www.mmsonline.com/articles/0305cnc.html

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site

FAQ559-1100
FAQ559-716

 

[diamondjim]

We in design engineering preferred drawing to the
max material condition. The shop insisted that we
draw to mean dimensions. The shop won. Both make
sense.

 

[fryed911]

...This way of tolerancing makes it easier for the designer do define the min. clearance/interference.
Say we have a shaft 50mm dia and we want a bore locate on it with the min. clearance of 0.1mm and the machining total tolerance for both parts 0.05mm.
The "metric way" to dimension it would be:
Shaft dia 50 +0.0/-0.05
Bore dia 50 +0.15/+0.1
Locating smallest bore 50 +0.1) on largest shafts (50 +0) shows immediately the min. clearance...

...the main reason for doing it is to give to BOTH parts the same nominal size and using the tolerances define the fit.

In this example the shaft is supposed to be 50mm diam. So, I would just specify:

shaft: 50.0 +/- .025
bore: 50.15 +/- .025

This would also make sense, since the machining error is "random" and can be "+" or "-". I assume this is why why fabricators would prefer mean tolerances.
Largest shaft (50.0+.025) in smallest bore (50.15-.025) shows min clearance of .1 as expected.

 

[drawoh]

1.250 +.003/+.001 DIA shows the real diameter of _MY_ scale model. I should have been clearer. You guys are making my point. There is more than one way to do this, including some dumb ways. I have gone into AutoCAD drawings and found dimensions exploded and typed. I guess the equivalent in SolidWorks would be to replace the <DIM> with text ("I'm in a hurry!"). I have not encountered this yet.

I prefer to model at the exact nominal dimension. The shaft and the hole are modeled at 1.250"DIA or 50mmDIA or whatever. On my arrangements or assemblies, I make a note indicating an ANSI fit like RC4 or LC5, depending on my requirements. Lately, I have been marking the ISO tolerance codes on my dimensions, making the tolerance independant of the current dimension. Modeling MMC requires me to know what tolerance I am using, and I am not always sure of this until late in the design. The ANSI and ISO tolerances vary with diameter. At the end of the job, I fix everything to make it readable to the shop, since they are the primary users of the drawing. I prefer to send drawings out to the fabricator, and I send DXFs if they ask me. I have sent SolidWorks models to sheet metal shops.

A corporate standard is desirable here.

JHG

 

[AndrewUK]

Quote:

In this example the shaft is supposed to be 50mm diam. So, I would just specify:

shaft: 50.0 +/- .025
bore: 50.15 +/- .025

This would also make sense, since the machining error is "random" and can be "+" or "-". I assume this is why why fabricators would prefer mean tolerances.
Largest shaft (50.0+.025) in smallest bore (50.15-.025) shows min clearance of .1 as expected.
-----------------------------------------------------------
I would agree with the above. I've been producing programs for milling and turning for over 10 years in the UK and we get drawing from all over the world.

We always standise them to nominal with +/- tolernaces.

It is far easier to control in production for especially on milling out thin materials where we cut out circuits in one pass.

Regarding +/+ tolrances we see these a lot on features such as push fit holes for electronic components, often drill diameters are specified 1.8mm Dia +0.02 / +0.5

 

[Tmoose]

"tolerance designations like H7/g6."

"I heard someone say that the drawing needs to minimize how much arithmetic the fabricator has to do. NO! That is part of the fabricator's job and it is expected that he will have to do it."

"At the preliminary phase of the design, I even use the ISO tolerance codes because they are independant of the dimension. I have not the nerve to send these out to the fabricator. "

"To be fair, though, the draftsman should never go out of his way to make a drawing that requires the machinist to figure things out!"
--------------------------------------

We used some moderately complicated power drawbars from a German company. They called out their required fits as H7/g6, etc. They also included a table translating those designators into real numbers.

I'll bet that saved a few re-works and non-value-added discussions about the difference between g6 and G6.
Well worth it.

 

[RedPen]

We outsource fabrication to a rather long list of qualified vendors here in the USA. Over time, the same part can be made by several different suppliers. We provide SolidWorks models (or 3D translations; IGES, STEP, etc.) and minimally dimensioned drawings to them. We receive better (more accurate) parts by modeling to the nominal/mean value and using symmetric tolerances as most of our suppliers CAM directly from our models. Force fits (and a few other special cases) being exceptions to this general rule. Fasteners and purchased hardware are always modeled at MMC.

For us, modeling/dimensioning a nominal value with either +/+ or -/- tolerances is the shortest path to rejects and scrap. When the modeled geometry and/or dimensioned print show nominal values outside of the allowable tolerance range we often get what we modeled/drew instead of what we wanted.

RedPen

 

[alexit]

I like to model at MMC nominal then use bilateral tolerance on the drawing to fit (i.e. shaft at 40 -.003/-.009 & hole at 40 +006/+012). This works with vendors that read the drawings and the guys using the model w/o checking the print still have enough stock to rework the parts when I send them back.

 

[AndrewUK]

I've always found Zeus to be hepful when quoted H&/g6 type fits they have the tables inside.

http://www.google.co.uk/search?hl=en&q=zeus+engineering+booklet&spell=1

 

[frans]

I was trained to the ISO drawing standard, but through experience learnt that:
It is OK to specify H7/g6 - you only have to reject a part once and then everybody knows. Sounds harsh - but heck, my time costs more than the guy on the floor and hence I only need to communicate my design intention, in this case a close sliding fit.

Each workshop is different. You first have to understand how a part will be made, then dimension it. What works for one workshop costs time in another - they have different tools and techniques.

Drawing is the way we talk to the guys on the floor. While the correct way is to give only the minimum dimensions, the best way is give some reference dimensions and mark them as such - especially for fabrications.

If you get things done on contract you better tollerance properly or you will have no comeback. However, use realistic tollerances - or it can cost you heaps.

 

[Plastserv]

As "BOO 1" correctly stated your dimension should be the target number. The tolerance is what size of deviation on both the plus side and the minus side creates an accptable part.

As far as how to show the tolerance formatted as you have asked depends on the cad system you use. I have SolidWorks. In the drawing mode it allows me to choose various methods of displaying the tolerance. You should choose according to your company standard if applicable, or whatever method most clearly shows your requirement for deviation.

 

[dparker213]

Dimensioning in this fashion is common to the company I work for when designing certain types of assemblies. We manufacture machine tools. Fits are very important and dimensioning in this way lets the machinist know what your intentions are.

For instance, lets say I wan't a cylinder assembly with a nominal bore of 10". I would dimension a class RC3 precision slip fit intended for a nominal diameter of 10 inches like this:

10.0 +.0020/-.0000" for the hole,
and 10.0 -.0025/-.0037" for the shaft.

This lets the machinist know immediately what the target assembly dimension is, in this case we are going for a nominal bore of 10.0".

The method that you are accustomed to would dimension these parts like this:

10.0010 +/-.0010" for the hole,
and 9.9969 +/-.0006" for the shaft

This would likely confuse our machinists as to what the intended result would be.

 

[ewh]

I understand the usage of -/- tolerances, but feel that if the dwg and design are correct, the machinist doesn't need to know anything about the assembly. I would use 10.0010 +/-.0010" for the hole and 9.9969 +/-.0006" for the shaft on the drawings. If the part is machined to those dimensions, the assembly will work.

 

[ctopher]

ewh, I agree.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ajack1]

Ehw I believe the +/+ and -/- dimensions came from the holes and shafts standards h7 and the like.

The reason for this is they are a standard so any shaft or bearing or anything from any manufacturer will give you a press fit, slide fit or whatever is required.

They are all based around a nominal size and the tolerances change as the nominal shaft or hole size changes. So to use your example it may do what you want but the hole would be in a different set of limits to the shaft, i.e. one is 10-15mm and one is 6-9 (the exact figures may not be correct) so your sizes would not fit say a h7 manufactured by another company.

Why change a standard that works perfectly well?

 

[ewh]

ajack,
I guess I don't understand your point. As in the example above, I have a 10" nominal bore and need a class RC3 precision slip fit. This calls for an H7 hole and an f6 shaft.
What is the difference if I dimension the hole 10.000 +.002/-.000" and the shaft 10.0000 -.0025/-.0037
vs
the hole 10.001 +/-.001" and the shaft 9.9969 +/-.0006"?The range of an acceptable part is the same, it is easier to accurately model, and those numbers mean the same thing anywhere in the world (as long as they understand inches)
It shouldn't matter where I have it made, if it meets those tolerances, it will have a class RC3 slip fit and will work.

 

[ctopher]

The same for inspection. Won't inspectors measure the part the same in any case?
I am on ewh's side.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ajack1]

Having re-read what you said yes you are right it would be the same, however I still don’t see the point in going away from a standard that has been around for years and works fine, what is gained?

Maybe I am just being grumpy, I got home tonight to find my house had been broken into.

 

[ctopher]

That's too bad. I have an alarm, a dog and a gun. No break-ins yet. Hope all is well.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ewh]

ajack,
I'm just going along with the times. The classification system for fits is excellent for design. However, in today's world, we have to document that design using solids on a computer. It is much easier to see how a design works when you have the parts modeled at a size they will actually exist, and document it as such. A +/+ or -/- tolerance adds confusion to this situation, i.e. a 10" nominal shaft should be modeled as it would be created, 9.9969 +/-.0006".
Sorry to hear about the break in. That's enough to make anyone grumpy.