What's new
What's new

Drawing/Model discrepancies disrupting our schedule

96Jack

Plastic
Joined
Mar 22, 2019
My shop keeps running into minor discrepancies between customer drawings/models, or drawings that are just missing little bits of information. Some random examples we've ran into recently-
  • Drawing calls for a .015 corner radius +/-.005 but it's modeled at .031".
  • Drawing calls out a true position to a datum that doesn't exist.
  • Drawing has a couple four-place decimal dimensions but the tolerance block only covers two and three place decimals.
  • Drawing says to use stock material but then they attach tight GD&T to the stock which is out of our control.
  • Hole sizes differing between drawing/model
We do our best to catch these things during quoting or programming, but a lot of times it doesn't get caught until we're in the middle of proving out our setup piece. When this happens we put the job to a halt and I reach out to our customer. Most of the time I can get a response within an hour, other times it'll take a full business day. Our machine sits in the meantime and every job scheduled behind it is potentially getting delayed. If we choose to move on to another job, then knowing my luck we'll get an answer 20 minutes later and we'd just wasted a several hour setup. If we choose to pause and wait for an answer, then the machine might not make chips all day. Seems either way is a losing scenario.

I guess I'm just wondering if this is normal and how other people handle these situations. Are there certain things that other shops take liberties on and make decisions about without contacting the customer?
 
I've experienced this before. Don't have a lot of good advice, except to say that in my experience, the drawing always trumps the solid model. Whatever is on the drawing is how you make the part, any deviations in the solid model are treated as mistakes and fixed to match the drawing. This should at least streamline the first and last issue.
 
My shop keeps running into minor discrepancies between customer drawings/models, or drawings that are just missing little bits of information. Some random examples we've ran into recently-
  • Drawing calls for a .015 corner radius +/-.005 but it's modeled at .031".
  • Drawing calls out a true position to a datum that doesn't exist.
  • Drawing has a couple four-place decimal dimensions but the tolerance block only covers two and three place decimals.
  • Drawing says to use stock material but then they attach tight GD&T to the stock which is out of our control.
  • Hole sizes differing between drawing/model
We do our best to catch these things during quoting or programming, but a lot of times it doesn't get caught until we're in the middle of proving out our setup piece. When this happens we put the job to a halt and I reach out to our customer. Most of the time I can get a response within an hour, other times it'll take a full business day. Our machine sits in the meantime and every job scheduled behind it is potentially getting delayed. If we choose to move on to another job, then knowing my luck we'll get an answer 20 minutes later and we'd just wasted a several hour setup. If we choose to pause and wait for an answer, then the machine might not make chips all day. Seems either way is a losing scenario.

I guess I'm just wondering if this is normal and how other people handle these situations. Are there certain things that other shops take liberties on and make decisions about without contacting the customer?
Ideally you should structure your process/procedures to catch these sorts of things *early* on, before they present a risk to schedule or profitability:

1.) During your RFQ/quoting process you should attempt to recognize features that may require tooling that may not be already on hand so that you can quote that into your part cost. Ditto for specials that may take time to procure. It's understood that you probably don't want to over-engineer your quotes, but at least catch the first-order ("big") things....

2.) Get clarification on ambiguous/missing details on the drawing/CAD data (again, this happens ideally at time of quote). A +/- 0.005" feature may require little care; but a +/- 0.0005" may require additional time, and therefore *cost.* Capture this up front to save heartburn later.

3.) I get it: sometimes you just can't catch everything right up front, but as you're programming the job these details should *all* be understood and accounted for. You may still have time to get last-minute clarification from your customer before the job hits the floor, but again: the later in your process you catch these things, the more risk to schedule & profitability they will present.

Our shop runs a mix of prototype/non-repeat jobs, as well as some production/repeat work, and our processes differ somewhat for each type. Much of the proto work is quoted/made from CAD data only, with a bit of verbal input as well. Where this presents risk to us (or the customer) we get clarification from the customer *at time of quote.* For jobs that seem risky we suggest incremental steps (sample parts, process experimentation, NRE charges, etc) in an attempt to remove uncertainty. We charge for this but recommend it when customers seem unsure of exactly what they want.

Believe me when I say that we suffer thru ALL of the items in your list! The key is to mitigate them wherever possible: "an ounce of prevention is worth a pound of cure" as they say!
 
I've experienced this before. Don't have a lot of good advice, except to say that in my experience, the drawing always trumps the solid model. Whatever is on the drawing is how you make the part, any deviations in the solid model are treated as mistakes and fixed to match the drawing. This should at least streamline the first and last issue.
Interesting perspective. We have a boilerplate note on our drawings that says in the event of a conflict the solid model rules as that is what was actually designed. And the reality is that 99% of the stuff we do the drawing has nothing more than a few views of the parts and maybe a couple critical dimensions and then notes on materials, finish, etc. You can't make parts from these drawings as there just isn't enough detail for that. But that is what the solid model is for... And then a lot of times for us it is a prototype so there isn't a drawing as of yet, just a solid model
 
Interesting perspective. We have a boilerplate note on our drawings that says in the event of a conflict the solid model rules as that is what was actually designed. And the reality is that 99% of the stuff we do the drawing has nothing more than a few views of the parts and maybe a couple critical dimensions and then notes on materials, finish, etc. You can't make parts from these drawings as there just isn't enough detail for that. But that is what the solid model is for... And then a lot of times for us it is a prototype so there isn't a drawing as of yet, just a solid model
You've just contradicted yourself in one single sentence!
On one hand you've said that "in the event of conflict the solid model rules ", and immediately followed by saying " drawing has nothing more than ... critical dimensions ..."
So what gives?
Every single RFQ I have ever seen from the likes of Boeing, P&W, Lockheed etc have always clearly and unambiguously stated that the governing document is the drawing, all other (not otherwise indicated ) dimensions are to be taken from the solid model with the following UOS criteria : ....
 
Not a contradiction at all. Perhaps I was not clear. The drawing has the key dimensions that we want measured in production, nothing more. Those dims come from the solid model but we only show those few we want inspected on the print. Solid model still rules, we just show them on the print for convenience and clarity in communications.

Was looking at a new print just today and we were scratching our heads to put even one useful dimension on it. The part (injection molded) has nothing useful to dimension on it that we could figure out. We ended up putting a couple overall ref dims on it to show the basic part size, but they are only reference (FYI) dimensions. So a part print with no real dimensions on it... Use the solid model to make the mold, not the print...as always, for us.
 
In the last ten years there has been a move to make the solid model the master. The drawing becomes an inspection document and not a thorough description of the part. It's nice to include some reference dimensions for overall size but, they should be marked as such. This is an attempt to recognize that everything is (or should be) done in CAM and a CNC. A note on the drawing for a small part (less than a foot) will likely say something like:

Parts to be manufactured using best shop practices. Dimensions to be +/- 0.005" to the supplied solid model, unless otherwise noted.

The intent is to free up the manufacturer. Profile the part using an endmill. Use the real diameter in the CAM. Cutter comp isn't necessary. Just use real values. Put the holes where the holes are in the model and make them that size. If they need to be a certain size (reamed or bored), they are called out with expected inspection limits. If they are threaded, the specification is called out on the drawing.

In theory, this should eliminate unnecessary things like ridiculous flatness and perpendicularity specifications. The only reason the designer is often forced to put stupid GD&T dimensions on a part is because someone will insist on doing them on a knee mill (not best shop practice) and they don't bother to check tram to the part.

The intent was never for a giant setup on a CMM, sweeping the cylindricity of a bore, finding the best fit axis, then checking squareness to a best-fit plane that it derived from dragging 80% of the flat surface. Just poke a straight hole using a real CNC machine and we're good unless the drawing calls out otherwise.

Surprisingly, this has not worked as intended. Either the engineers don't understand things like drill sizes, or machinists continue to do parts the lazy way. One of the last ones I experienced was 100% laser scanning and certification of the part. Manufacturing insisted any dimension that was sub 0.010" was to be scanned and checked in their inspection software (their own internal process). Even after all that, the parts were pure trash.
 
Not a contradiction at all. Perhaps I was not clear. The drawing has the key dimensions that we want measured in production, nothing more. Those dims come from the solid model but we only show those few we want inspected on the print. Solid model still rules, we just show them on the print for convenience and clarity in communications.

You have got to be kidding me!!!

The drawing has the key dimensions that we want measured in production, nothing more.

Which means PRECISELY THAT THE DRAWING is the governing document!!!

To put it more bluntly, if the drawing says .500 +.005/-0, the model is drawn to .500 and the RFQ says UOS +/-.005, then please tell me what document rules?
How exactly do you differentiate on your model that a hole is a slip fit for a 5/16 dowel, press fit for the same dowel or that it is a clearance for a 1/4-20 bolt?
If you say that you will model it to the exact diameter you need I command you, but you still need to differentiate from other hole features having a UOS tolerance!

IOW model is boss unless the drawing says otherwise!
 
Great! Another one contradicting himself in one breath!

First this:

In the last ten years there has been a move to make the solid model the master. The drawing becomes an inspection document and not a thorough description of the part.

And then right after:

Parts to be manufactured using best shop practices. Dimensions to be +/- 0.005" to the supplied solid model, unless otherwise noted.

The hell with Venus and Mars, some among us are from another galaxy!
 
How is that contradictory? The solid model measures 6.000". I can hit that number all day long */- 0.005" without measuring a thing. Maybe I check a few dimensions to make sure the end mill hasn't broken and I move on.

Edit: Haas used to come to the trade shows and pump out sample parts all day long while showing machines to the public. Those parts would all pass that inspection. You can measure the demo parts and see obvious dimensions are obvious: 0.251, 0.124, 1.499. Those were throw-away parts.
 
How is that contradictory? The solid model measures 6.000". I can hit that number all day long */- 0.005" without measuring a thing.

Yes, I bet you can!
But!
If the drawing tells you that the 6.000" hole is a fit for an xyz bearing, I bet you fuck the thing up and do it again!
 
Yes, I bet you can!
But!
If the drawing tells you that the 6.000" hole is a fit for an xyz bearing, I bet you fuck the thing up and do it again!
The drawing would have a call-out pointing to that hole. It would call it out 5.9970-5.9985" (or whatever it would be for one that big) and have a flag note saying it's a bearing press fit.

When I sit down to program the part I would look at the drawing, notice it only has a few call-outs and say:
  • I see a call-out for a 1/4-20 UNC tap through, 6 places. I guess I need a 0.201 tap drill and a spiral point tap.
  • There's a few callouts for for 0.2490-0.2495 and a note saying dowel pin press fit. Guess I need a 0.2490 dowel pin reamer and a C or D drill to start it. They're dowels so I'll use a stubby drill to make sure they're right.
  • The fit on that 6" bearing is gonna' take a boring head for these called out tolerances.
  • Those 0.257 holes on the model don't have any call-out on the drawing. They must be clearance holes and need an F drill. Oh, look at that: F is exactly 0.257. This person knew what they wanted.
Using current methods, a no-skill machinist or overzealous inspector looks at a three place hole dimension at 0.257" and thinks he needs to sweep the bore on a CMM. Using ANSI standard, I can't point to the hole and say F because that implies drilling and ANSI says you can't specify the process. All anyone wanted was a clearance hole.

Tapped holes look just like dowel holes unless they're beaten to death with GD&T. Some inspector will milk a day checking tapped hole locations. The machinist too lazy to find the F drill punches them 1/4" and says they're "within tolerance." Then the parts don't work and the engineer gets blamed.
 
These arguments are exactly why I hate it when the customer supplies a model and a shitty drawing or no drawing at all. Or a model with notes on critical dimensions. Maybe this is common place in some types of work, but not in the type of work I do. I'll also say my work has little surfacing and litte detail that can be "whatever" it comes out.

CAD has facilitated the dumbing down of designers. I do not mean CAD is bad, but that it can be poorly used. Very poorly used indeed. The manufacturer should not be the defacto design/drawing checker!

If my customer consistently supplies conflicting info that impacts my profitability, I charge them more. If my customer seeks my help with the design, I charge more. The customer that always supplies good data gets the best price.

How do I know if a close tolerance feature is modeled at LMC, MMC, or nominal or anywhere in between? Well, I don't unless I check it against a drawing. "Just cut it to the model" may or may not create a useable part. An unuseable part makes me look bad and doesn't help my customer.

If the new normal is conflicting part data I want none of it. I've only got a few more years to go so I'll fire those customers that expect me to read their minds and second guess their designs and tolerances. It's not worth it!
 
Interesting perspective. We have a boilerplate note on our drawings that says in the event of a conflict the solid model rules as that is what was actually designed. And the reality is that 99% of the stuff we do the drawing has nothing more than a few views of the parts and maybe a couple critical dimensions and then notes on materials, finish, etc. You can't make parts from these drawings as there just isn't enough detail for that. But that is what the solid model is for... And then a lot of times for us it is a prototype so there isn't a drawing as of yet, just a solid model

Interesting, thanks for sharing your experience. It seems based on what Donkey has said that things may be changing and I'm not keeping up with the times.

Though I guess all this simply creates more confusion for the OP. All I will say is that I have found many times more mistakes in solid models than I have on drawings, provided the drawings are intended to be used to make the print, and not non-technical sketches such as dstig is describing.

I guess at the end of the day, it is best to establish with the customer up front whether the drawing or the model is the "master" document.
 
Sometimes we get a drawing that does tell us.

NOTE: 6

REDUCED INFORMATION DRAWING. ALL DATA SPECIFIED ON THIS DOCUMENT HAS
PRECEDENCE OVER THE SOLID MODEL FILE. ALL UNSPECIFIED DATA IS CONTROLLED
BY THE SOLID MODEL FILE.
 
I think you need both (most of the time), and there ought not be a "Master". They should not conflict, and if they do it's an issue that needs to be cleared up.

The drawing expresses things that the model cannot (or, at least, never does IME), like thread specs. For virtually all of the parts I make that have threaded holes, the model just has a hole with the minor diameter (that usually goes deeper than the thread needs to), say, 3.3mm for an M4. Then the drawing calls out something like "M4X0.7 - 6H [down symbol] .25".

The model, OTOH, defines the geometry for non-trivial contours that a drawing cannot (reasonably), and all of the various sundry dimensions of the part that would make a drawing overly complicated. Something like this, that I'm working on today:

Part.png

If the drawing had to call out dimensions for every single contour, it would be super-busy and hard to read.

The drawing says, "REFER TO ASSOCIATED SOLID MODEL FOR FULL GEOMETRY." Great, that's easy. It does NOT say, "Drawing wins" or "Model wins". They both win :cheers:.

Regards.

Mike
 
My shop keeps running into minor discrepancies between customer drawings/models, or drawings that are just missing little bits of information. Some random examples we've ran into recently-
  • Drawing calls for a .015 corner radius +/-.005 but it's modeled at .031".
  • Drawing calls out a true position to a datum that doesn't exist.
  • Drawing has a couple four-place decimal dimensions but the tolerance block only covers two and three place decimals.
  • Drawing says to use stock material but then they attach tight GD&T to the stock which is out of our control.
  • Hole sizes differing between drawing/model
We do our best to catch these things during quoting or programming, but a lot of times it doesn't get caught until we're in the middle of proving out our setup piece. When this happens we put the job to a halt and I reach out to our customer. Most of the time I can get a response within an hour, other times it'll take a full business day. Our machine sits in the meantime and every job scheduled behind it is potentially getting delayed. If we choose to move on to another job, then knowing my luck we'll get an answer 20 minutes later and we'd just wasted a several hour setup. If we choose to pause and wait for an answer, then the machine might not make chips all day. Seems either way is a losing scenario.

I guess I'm just wondering if this is normal and how other people handle these situations. Are there certain things that other shops take liberties on and make decisions about without contacting the customer?
#2, #3, and #4 can and should be cleared up with the customer early on before you start coding or proving anything out or get any machines tied up.

#1 and #5 can be caught in CAM with whatever "Verify" functionality your CAM has. Again, no machines tied up yet.

If your customer repeatedly does this stuff, I would have a chat.

Regards.

Mike
 
I think you need both (most of the time), and there ought not be a "Master". They should not conflict, and if they do it's an issue that needs to be cleared up.

The drawing expresses things that the model cannot (or, at least, never does IME), like thread specs. For virtually all of the parts I make that have threaded holes, the model just has a hole with the minor diameter (that usually goes deeper than the thread needs to), say, 3.3mm for an M4. Then the drawing calls out something like "M4X0.7 - 6H [down symbol] .25".

The model, OTOH, defines the geometry for non-trivial contours that a drawing cannot (reasonably), and all of the various sundry dimensions of the part that would make a drawing overly complicated. Something like this, that I'm working on today:

View attachment 416302

If the drawing had to call out dimensions for every single contour, it would be super-busy and hard to read.

The drawing says, "REFER TO ASSOCIATED SOLID MODEL FOR FULL GEOMETRY." Great, that's easy. It does NOT say, "Drawing wins" or "Model wins". They both win :cheers:.

Regards.

Mike
This is a perfect example of what can go wrong. A customer wanted me to make some small potting molds from Delrin strictly using the Solid Model, no actual drawing. I advised against It and they Insisted on proceeding anyway. When all was said and done there we're (6) # 6-32 threads tapped In one side of the molds. Turned out those were supposed to be Heli-Coiled. But no way of telling that from just the Solid. Had to bring those back In re-drill and Heli-Coil them. Not the end of the world. But still cost time and money.
 








 
Back
Top