Tolerances - Undimensioned Drawings 2

[MechDesignR]

I am designing several new brake formed parts that are defined on undimensioned drawings with a +/- .030” general tolerance. I am not sure if the interpretation of this general tolerance is the same across the aircraft industry (seems like it should be). I need to know the correct interpretation since I have hole patterns used to attach purchased parts and I need to determine the required tolerances to ensure interchangeability. I don’t want to add dimensions to hold things tighter than the general tolerance unless actually needed. Additionally, we don't use GD&T (even though we should).

First, considering just a flat part, is my understanding that tolerances do not build-up, in other words, the tolerance between two holes would still be +/- .030” and the tolerance on the length of a part would be +/- .030”. If that is the case, then an undimensioned drawing is actually holding tighter tolerances than a dimensioned drawing with 2 place dimensions (because it would be like having every possible relationship dimensioned, really over-dimensioned). Is that right?

Second, what is the interpretation when bends come into play – is there an additional tolerance on the location of each bend? I assume you would have to at least add the angular tolerance (+/- 2 degrees) to determine the tolerance on the length of a part that has several 90 degree bends?

Third, Is the flat pattern inspected before forming and the final part inspected again after forming? Does anyone have first article inspection experience with sheet metal parts? I have heard several conflicting opinions - does anyone work at a company that has an official document to clarify the interpretation of undimensioned part tolerances?

Thanks,
MechDesignR

Atlanta

 

[der8110]

you might be trying to read more into this than is actually there. Yes the part should be inspcted at the flat pattern stage. Scaling of the drawing is the important factor; basically the flat part and then formed part are held up against the full scale plot and compared. This is commonly done when tolerancing is not critical or mating features are accomodated on assembly.

Or used when lazy.

 

[IRstuff]

Seems to me that you make too many assumptions about how the supplier is going about his fabrication. If you don't control critical dimensions, then they will be uncontrolled, and you and they will arguing about the problem later on when things don't fit.

The bottom line is that if you have something that needed to be controlled, and you didn't specify the degree of control, your company will probably lose the argument and eat the cost of anything that was nonconforming to an unspecified requirement.

TTFN

FAQ731-376

 

[tbuelna]

MechDesignR,

Engineering drawings typically define the requirements for a finished part as shown on the drawing. With formed sheet metal parts it is common to define a flat pattern layout of the part with mold lines, bend lines, etc. It is also common with digital CAD designs to employ "reduced dimension" drawing formats. Where the dimensions and tolerances are defined by a general note or specification, unless otherwise specified on the drawing.

If you need to control the location of a feature like a hole pattern to ensure that the mating part will fit, then you need to put the necessary dimensions and tolerances on a drawing that defines the finished part condition.

The FAI spec for the aerospace industry is AS9102. The FAI is a validation of the part as defined on the drawing. If the drawing defines a flat pattern, then that's what will be inspected.

Good luck.
Terry

 

[MintJulep]

I am designing several new brake formed parts that are defined on undimensioned drawings

What is an undimensioned drawing? How does anyone manufacture anything without dimensions?

with a +/- .030" general tolerance.

Is +/- .030 acceptable for the part you are designing? It's YOUR job as the designer to define the tolerances that are required to allow the part to function properly. The person that typed .030 in the tolerance block of your standard drawing border had no idea what you would be designing today.

is my understanding that tolerances do not build-up

No, that's wrong.

 

[mfgenggear]

Gentlemen

Possible reason.
some drawings where giving basic configuration,
why because it was controlled by a master mylar.

this was done when there where two or more parts being assembled together. drilled & rivited, or bolted.
all the holes where drilled by slaping a mylar up against the assemly & drilled with pilot holes then held in place with clicos(temperorary fastening). to verify edge distance then finished drilled.

check with the assembly if the holes are prematurely drilled it will not match the other details.

if this is not the case the GD&T should be used.
parts should be drawn & tolerance in the formed view.
then it's upto the the vendor to hold the flat pattern.
it is easier to match drill instead of trying to hold super tight true positioning.

HTH

mfgenggear

 

[rb1957]

ok, you're designing a part that probably had a mylar master, and wondering how to dim'n the hole pattern ? why not look at the mating part (a brake ?) to see how it's pattern is dim'ned ?

personally, why inspect the flat pattern ? aren't you most insterested in conforming the final part to the eng'n ??

 

[KENAT]

"I am not sure if the interpretation of this general tolerance is the same across the aircraft industry (seems like it should be)."

Does the drawing refrence a spec for drawing interpretation? ASME Y14.5M is the most common spec in the US. If no drawing spec is given then it's debatable if the interpretation would be the same. In practice the interpretation would probably be similar to 14.5, however that's not legally binding.

"First, considering just a flat part, is my understanding that tolerances do not build-up, in other words"

Wrong - though depending on how the part is dimensioned you may think it's true. The tolerances are applied to the dimension. If say a 2 hole pattern is dimensioned from an edge to the first hole, then another dimension from first hole to second then no stack up between the holes. However, if dimensioned from edge to first hole, and edge to second hole, then you get a stack up.

As mentioned, drawings generally define the finished article and that is what is usually inspected.

+-.030 is a large tolerance for hole patterns, while you'd need to do the math and /or take into account match drilling, it's likely too large.

When you say undimensioned drawings I take it you are using hybrid model/drawing definition as tbuelna says. You still have to fully dimension it somehow. Variability in how +-.030 might be applied/interpreted is one problem with trying to do this too simplistically.

Honestly, it seems like you don't have a firm basis in dimensioning & tolerancing. I suggest you get hold of the 14.5 standard (assuming that's what you work to) and learn some. Also forum1103 may be a good place to ask questions, though they/we can get a bit pedantic.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[mrainey]

If you had a row of eight holes, with each hole being dimensioned from the previous hole, the total length of the hole pattern could vary all over the map. If each hole was dimensioned from the same edge, you would lock down the location and control the total length variation.

Software For Metalworking

http://closetolerancesoftware.com

 

[ewh]

The only way to avoid dimensioning it that I know of is to invoke a blanket profile tolerance. This is not ideal, as the holes should probably be more tightly controled than the edges, but that is just a guess.
Technically this is not a complete drawing, and scaling from a plot is usually forbidden unless the plot is stable (on mylar) and verified for accuracy.
Just my 2 cents...

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[mfgenggear]

missing the point.
match drilling to a mylar was a an old school method of manufacturing & far as I know it is used today.

it gets very difficult to match up more than 3 or more assemblies.
it has been done this way for decades.
the drawing should specify to a master model & mylar.

the main concern is edge distance from holes & edges.

how ever if this Detail is a single piece of hardware
that assemple to one other detail then true position should be good.

HTH

MfgEngGear

 

[ewh]

It is a simple matter to verify a mylar plot before using it for drilling.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[uGlay]

i know some boeing drawings come undimensioned and with a 10"x10" grid throughout so you can scale off of them. they do come with flat patterns and the concensus here is that if needed, the parts can be formed on-site in case repairs are needed.

typically we reverse engineer those and insert them into our own drawings, add our own tolerances which are:

0.000 +/- 0.005
0.00 +/- 0.010
0.0 +/- 0.030

we never send out ANYTHING undimensioned, and even though we model everything parametrically, we also never have parts mastered off STEPs/IGES. so yeah we have to dimension every feature of every part. STEPS/IGES only go out as 'reference only' mostly for the programmer/machinist in case they want to pull off some weird dim off of it. sending undimensioned drawings is out of the question as our suppliers would do 'whatever the hell they want' and at the end it would bite us in the arse big time.

as far as what to dimension and how many decimal places it ends up being at the discretion of the designer/detailer and based on application, machine shop capabilities, cost and most importantly experience.

SW2010 Premium SP0.0
Intel Core 2 Duo CPU
2.2GHz, 2.00GB RAM
QuadroFX 3700
SpacePilot

 

[ewh]

uGlay,
I can understand avoiding iges for machining purposes, but why step? We often use it for a variety of tasks where the native file (or a parasolid) is unsuitable. We do a model verification (comparison) after translation between the native file and the step, and have yet to run into any problems.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

ewh, I think uGlay is just saying they haven't gone the MBD route yet in any way shape or form.

To the OP, I suggest you take a look at ASME Y14.41, it's not particulary user friendly or usefull but at least it's a start for Digital Product Drawing/Model Based Dimensioning (i.e. product documentation based on model with no or incomplete/simplified drawings).

There have been several good threads on MBD over in GD&T and elsewhere in the last few years.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[uGlay]

ewh:

model verification is fine, but sending a STEP to a machine shop and telling them to do it... dont know about that.

SW2010 Premium SP0.0
Intel Core 2 Duo CPU
2.2GHz, 2.00GB RAM
QuadroFX 3700
SpacePilot

 

[ewh]

If caveats are included as to tolerancing of critical features, it can work; we do it quite often.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[MechDesignR]

Second Try

Most of the responses to my question were way off target. I will try to explain more carefully exactly what I am looking for. First, I am working for an aircraft company that uses “old school” undimensioned drawings to define brake formed sheet metal parts (the same way things have been done for many decades). These undimensioned drawings go by different names at different companies: PCM, EMD, Mylar, Undimensioned Master, etc. Typically, these “undimensioned” drawings define a flat pattern, show bend centerlines, specify bend angle, direction and radius. They only contain dimensions for features that need to be held tighter than the general tolerance of +/- .030”. For example, full size fastener holes would have a diameter dimension. If you aren’t already very familiar with this type of drawing, your reply will not help at all.

Where I currently work, undimensioned drawings have a general tolerance of +/- .030” with a note that states “no tolerance accumulation is implied in any series of features”. Some people understand this to mean that the length of the part (scaled off of the mylar or measured in cad) would have a tolerance of +/- .030” and similarly, the distance between the centers of two holes would be +/- .030”. Other people interpret this to mean that one edge of the part is held to +/- .030” and that the location of a hole is held to +/- .030” and that the length of the part would have a total tolerance of +/- .060” and similarly, the distance between the centers of two holes would be +/- .060”. The correct interpretation is important since I am designing new sheet metal parts that will mate with purchased parts (things can’t be drilled at instl) – I have to ensure interchangeability by calculating the tolerance needed for my hole pattern. Sometimes a general tolerance of +/- .030 will work for the hole pattern (due to floating nutplates and large holes) and no dimensions are needed. While other times a tighter tolerance is required.

Apparently, the interpretation of undimensioned drawing tolerances varies from company to company. I would like to hear what other people in Aerospace have to say – what is your understanding of the general tolerances on undimensioned parts? What statement is used on the drawing or elsewhere to clarify things? Maybe someone who makes or inspects these parts could shed some light on the subject?

Thanks!


Atlanta

 

[KENAT]

Not sure how much more you'll get here, you may want to try forum1103 with your clarified question.

If you do post there I suggest you put a link back to this thread. (thread2*266252 but replace the * with -, just as shown near the top of the screen under the title)

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[HANDCALC]

MechDesignR,

You've asked a very good question, which involves as much "human dynamics" as it does "drafting standards". When working as an MRB Engineer for Boeing, we found that mylar drawings frequently showed the same part in different zones, and that drawing ADCN's were not always incorporated into all views on all sheets properly. In the end, the mylar drawings could be differently "interpreted" by QC depending on what zone and sheet was used as the inspection standard. To get around this sheet metal "check-fixtures" were manufactured, where the part was held against an edge, or snapped onto an inspection pin that picked up on a tooling or fastener hole. Periphery tolerance was scribed on the check fixture.

As a mechanical designer - you must check with the Quality Control department on how they inspect the parts you are mating with. Against the drawing or a check fixture? Sometimes this information is included in the Manufacturing Plan or Travellor..

Good Luck