What's new
What's new

Machining & Verification

lspotts38

Aluminum
Joined
Mar 7, 2012
Location
Northcentral Pennsylvania
Bit of a rant/looking for information here. I consistently find myself/processes that I have developed at the mercy/subjectivity of the inspection processes that are applied to the produced parts. I’m pretty sure that everyone that is here (in the forum, reading this thread, gives two craps about what they make) and is reasonably sure that what they make is a good part. My current issue is with the shifting application of part verification. I’m currently split between make it to the print, and I’ll make it the same every time.

Bit of context, issue number one was a drill point calculation, I figured a drill point a for a 118, drill was 135. Drill depth dimension was to the shoulder, as a practice we have been setting drills to the tip, so the P/A becacme important. Result was scrapped parts, the drill depth at full diameter was deemed to be be important, and the drilled depth ended being too deep by .050 on a .328 diameter. Was supposed to be verified by an inspector secondarily, he misinterpreted the drawing and ended up not catching that the drill depth was too deep. I’ll share some responsibility on this one, I miscalculated the depth based on a different point angle. But, I’ll also say that given a 135 degree P/A, the calculated drill depth would have still been out of spec based on the drill point length advertised by the drill manuf (standard hi-perf drill GP drill from Sandvik), something they do also reduces the effective point length. Issue is to me that the feature was to be verified secondarily, was mis interpreted and was not evidient until part specific gaging was available.

Second example is same part, different feature. Feature is a casting location, casting locators as related to machined features. Casting roughly concentric to a round cast feature, with the secondary and tertiary locators having an offset to the implied axis of the casting. Casting location was called to the secondary and tertiary locators specifically. Near as I can tell, what ends up happening is that the CMM needs/wants a primary datum to call out to given the absence of a specified primary datum, and has to construct a “perfect form” primary datum to calculate the dimensioms to the secondary and tertiary locating points. Casting location is positional of .060, and it appears that the primary datum being more than .010 out of flat negatively affects the positional accuracy, given the projection of the secondary and tertiary datums from the “A” datum, which IMO is way tighter than the .060 allowable to the secondary and tertiary.

Rant on. All of the drill point depths were within .001, probably less than that with the accuracy of the gaging method. After fixing that, I was inconsistently getting a position of cast features to machined, and didn’t understand how the CMM was <seemingly> arbitrarily referencing a phantom measurement and application of the primary datum to other measurements, even tho they were not specified, nor were included in the specification for the features that were measured “out of spec”. So I’m of the position that I will make the part the same every time, which I have demonstrated given the drill point case (incorrectly, exactly wrong) to the application of datum specification (not wrong, but not given all contributing factors).

Rant off. I need a sanity check. Five axis parts, two operations. Fairly significant quantities per year, not automotive but more than job shop. I don’t intend on making mistakes on drill point calculations on one tool of the 40 tools per part across 30 machined that are of similar conplexity, I think it happens. I also dont think I should be needing to delve deep into the datum plane construction of PCDMIS, but they had similar escalations of non-conformance. What do some of you guys do? I don’t have a problem with admitting and fixing an issue, given some reasonable investigation as to the justification of the original decision, but dammit if I’m not getting sick of changing machining programs based on changing inspection methodologies.
 
First and foremost, the CMM alignment issue. Note that castings are not something I deal with that often so others might have more useful insight.

You are doing a best fit alignment on the casting, when the actual machining is located from three reference points, is that right? Seems like that's asking for trouble to me, I can't see how you would get any kind of consistency part to part.

For the purposes of inspection you need to define a datum that you can accurately and repeatably pick up from some basic machined features (two or three holes and a plane that are all machined in the same orientation/setup for example), provided that suitable machined features actually exist on your part. You can offset that datum to match the drawing datum afterwards if necessary.

When that's established you can measure the locators themselves to see if they are within acceptable position.

As for the drill, yes that's on you, but you know and accept that. Most premium manufacturers publish the geometry of their drill points, Sandvik included.

For example (just a random selection): 460.1-0830-042A1-XM GC34
Point length is explicitly stated as PL.
 
IMO, the drill dia. being too deep is all on the setup guy. He just runs off the first pc, hands it to inspection and says "Is this any good?" WTF.

"Part specific gaging" for a drill depth? You mean a gage pin? If you're trying to hold +/- .005 on a depth then everyone needs to decide how it's going to be checked so everyone one is on the same page, but missing it by .050 and then running the whole lot?

As far as the casting datums, I'd have to see the print to offer any advice. I've seen a lot of good parts check bad because the CMM guy didn't align things properly. Also, your workholding should hold on the casting datums.
 
CMM program should pick up off targets similar to what you do in the machining fixture. If not you will chase your tail. Parts might be good either way, but you won't know. Moreover, it sounds like the CMM program alignment is whacked. I have fought alignments time and time again. Both internally and with our customers. I have never seen a program that was correct the first time around. Best way to prove or disprove what is going on is to do some indisputable open plate inspection. There is not any computer voodoo to get in your way. It's good or it isn't. You will hit, or may have already a time in your career where you know what you are capable of hitting tolerance wise without any inspection to know. I had a part the other day, the customer CMM'ed them and told me I was out by .04" on a set of features. I had a hard time keeping from laughing while I started to explain to them on the phone where there CMM operator had made an error misinterpreting a poorly dimensioned print. I was confident I was sub .005" as I would have had other trouble, turns out once changing the inspection method, I was sub .002".
 
Yeah, I am aware that I should have checked the drill depth some other way when developing the process. Interestingly, the drill shoulder depth was to have a process dimension of +/-.005 given some tolerance stackup, and I drew up a flush pin gage to check it. Things happen, get pulled onto other issues, was waiting on other tooling to arrive, proving out other operations & parts, time goes by and I never went back and checked the hole. Gage shows up a couple months down the road, and the hole is drilled too deep.

RE the casting datums, there was concern as to the rigidity of the primary datums, and given that concern, we and the workholding engineers thought it would be a more robust process to "translate" that datum to another more substantial surface and understood that some minor adjustments may be required in the future. Envision that the primary targets were located on an 1/8" thick aluminum cooling fin projected 2 inches out from a cylindrical 3/4 thick tube, we felt that it would be better to pull down onto the tube than onto the cooling fin. Unintended consequence was that when the primary datum plane moved away from nominal by a little bit, it greatly affected the measurement of the secondary and tertiary locators, and it took alot of digging to get to the root cause of the non-conforming dimensions.

I'm really trying to do better. Started doing an Excel sheet that breaks down all of the features of the part, lines them out individually. I try to check as much as I can, and lines out what I cannot verify (i.e. tolerance of position, unavailable gaging, etc) and pass it on. Been slowing down, trying to verify everything, yada yada. The part that had the issue has 373 line by line features that need verification. It's tough, given all the information that is out in the world, trying to work with people that give you suspect feedback, and seemingly small errors like drill point calculations bite hard. Stupid things like calculated a drill at 118 degrees, advertised as 140 degrees, and point length that is different than what the rule of thumb calculation would be for 140 degrees.

I know alot of people have to go through the same thing, any other ideas on how to eliminate that single line miss?
 
Double and tripple checks, i like the age old take a print and check dimensions and then go over them with a high lighter, its old school but its sure is simple and non highlighted dims become ever more obvious. Equally doing this stuff when your heads in the right place matters too, this is not the job to do late in the day.

As to casting datums, good luck with that, its a can of worms that just is near bottomless. You probaly need to be doing pre casting random inspections to try and cover your ass, even if that is at your own expense.
 
Pretty much everything everyone else said. There should be no hurry or "too complicated" or "too involved" in a First Article Inspection. (or second). People in the Industry have a bad habit of thinking they know everything (myself included). It is important to be perfectly clear about print interpretations and they need to be clear across the shop, including QC as Booze pointed out "everyone needs to be on the same page". If there are questions or questionable things---ask other people until everyone agrees. AND without exception, no one makes another chip until a proper First Article Inspection is complete and signed off.

As for the CMM, get a known good part, and set-up off that. If you get QC starting to use their imaginations you're fucked. Theoretical Datums and compound Angles from un-established planes and shit will screw you so hard it'll make you want to be a Politician instead. I do what Husker recommended before it even gets up on the Rock, I Inspect and verify every Feature and Dimension I can with Mic's and Indicators and proper hard Gauges, and when it's all done and there are only 3 Profiles to check then it goes to the Rock and CMM. Highlighter works wonders too, you begin to see a pattern there, it's almost comical. One Red one Green. Don't be afraid to red-line your print, putting the part on the back burner for an afternoon is WAAAY cheaper.

But most importantly, more than anything----if you missed it, you missed it, bite the bullet, suck it up, we've all done it. It usually just takes one good one to be very mindful, but it happens.

R
 
I love it when the cmm guys say its scrap, we say "you sure, run it again" and get different scrap numbers.

I don't believe them when they say its bad, don't believe them with they say its good either.
 
My favorite is when you supply a batch of parts, and they pull few pieces, sit on them for a few weeks, then inspect them and say they are bad. Upon investigation the other parts from the batch all assembled without hassle and went out the door already. After deeper investigation, the print isn't understood by anyone other than the engineers and machinists who make the parts, and the receiving inspection method was just a pair of calipers and the inspector was the shipping and receiving guy, who doesn't even know the difference between a dial caliper, digital caliper or vernier.

See this all too often.

Then my all time favorite is when you are asked to make x for y price. So you have to cut corners and cost everywhere you can, eventually you have a process which is cheap and effective, but ultimately 75% of the print dimensions are slightly out of spec or use 125% of the tolerance allowed... You follow the parts through the rest of their process and understand what every surface or hole interfaces with and know with a certain level of accuracy what you can get away with. Give a little here, take a little there. Once you go through all of this, it's darn near impossible to rein it back and make fully compliant parts, but after years and years, engineering still seems to think we make nominal parts and they forget the pain we went through just to get where we are cost and quality wise and after showing them copious amounts of data, they still won't open up the tolerances.....
 








 
Back
Top