Tooling pins on CNC

[CNCMAN172]

I have a few questions on using a CNC machine to cut holes for tooling pins. A friend purchased a Chinese CNC machine to setup a small sign business. He got Artcam to design the signs. Well when the CNC machine from China showed up it was very poorly built and not accurate at all. It appeared that it was built using a drill press and a band saw.

Anyway after we looked over the machine closely he decided to have a local shop machine new aluminum part for the machine.

He did all the drawing in Artcam and asked me to cut them on my small home made CNC out of MDF. They seemed fine so he setup the files to post to a Haas VF2. The machine shop provided the preferred feed and speeds and depth of cuts.

Well the tooling pins used were 4mm and they came out really lose on the Hass. I tested some tooling pins on my home machine and they felt good in plastic but when I tried them in aluminum they were way too loose.

We also discovered pretty much all the pockets for bearing were also loose.

What are we doing wrong we checked his files but importing the DFX file into Autocad LT and the diameters are all correct.

We measured the end mills which were all carbide. They were all exact or maybe .001" under.

We did not put in a finish pass but it seems to work in plastic. Comments welcome

[Geof]

Very often the exact same program on the same machine will give slightly different results in plastic than metal. I have found this and I figure it is just that the plastic can deform slightly under the cutting load so any holes end up slightly below size.

But whether or not this is the reason for your rresults I think just writing a program with 'correct' dimensions and then trusting it to give the desired size is a bit optimistic. This is the reason the machines have a "Wear" value to tweak the final sizes produced.

[CNCMAN172]

Thanks Geof,

I just find it strange that in the past I have cut small .125" tooling pins in aluminum and they had a very good snug fit. On a HAAS which is known for precision I am surprised at the loose fit. We even ran an experiement and drill a hole for a tooling pin just undersized and the tooling pin would not fit in the hole. Then we had a small 1/8" endmill enlarge the hole with a pocket command so it was cutting very little material. This technique also resulted in a hole far too loose for tooling pins.

I am especially surprised when I measure the carbide cutter with a Mitutoyo caliper and it appears to be as the manufactured lists the tool about .001 undersized so it was 0.124". Pretty surprising to see an undersized tool cut an oversized hole.

We even ran an experiment and had the machine shop post the test holes using Mastercam and it resulted in the same oversized holes. This does not appear to be related to the gcode. The tools did not appear to chatter as they cut these small holes so I am a little confused over the results.

It was pretty disappointing after spending $100/hr on a HAAS to have this kind of fit. The whole idea of having the machine shop to this work was to make sure his machine would have very good tolerance something close to .001"

Still scrating our heads.

[Geof]

Originally Posted by CNCMAN172 T.....I am especially surprised when I measure the carbide cutter with a Mitutoyo caliper and it appears to be as the manufactured lists the tool about .001 undersized so it was 0.124". Pretty surprising to see an undersized tool cut an oversized hole.....

You were plunging straight in, not interpolating with a small cutter?

It can be possible to get an accurate hole just plunging but it is necessary to drill a pilot hole first. Without a pilot hole a milling cutter ground for end cutting will tend to deflect and wobble around the center web. Have a look at one of these cutters and you will probably see that the cuttings edges on the end are not the same length. This means the cutter tends to get deflected when plunging due to the cutting load being uneven. Using a pilot hole balances the cutting forces because each cutting edge has the same engagement.

However, the cutting must be running very true, even a 0.0002" runout can result in a noticeably oversize hole when dealing with small sizes.

[CNCMAN172]

Geof,

These were single ended cutters and you are correct they can potentially wobble slightly but the way the CAM programs produce the G-code they start the hole well inside of the diameter and move down at .015" increments using ramps. Then as soon as the hole is at depth they do a helical down the entire hole at the correct diameter. This method I would think would yield pretty accurate results because during the final pass it is removing very little material and it is using a helical downward path so not real plugging at all during the final cut.

Again, all ideas and suggestions are welcome. I think in the future drilling these type holes and then using reamer would be much tighter. However in cases like bearings where you pocket them that would not work. Very stange to see these oversized.

Your comments on runout are correct but the Haas VF2 was using a 1/8" bit only 1" long in a collet and I would image the runout in that case is so small it would be hard to measure. Still the hole was worse on the Haas than it was on my homemade cnc machine while cutting aluminum.

CNCMAN
Russ

[Geof]

Okay you were interpolating them which only leaves the excuse of incompetence on the part of the Haas operator. Or at least that is my humble (not really) opinion.

Drilling, then bore undersize to make sure the hole is truly positioned (drills can wander) then ream may be the best for pins.

Bearings hole it should be possible to interpolate on a correctly programmed Haas using tool compensation so wear adjustment can be used to get to a precise size. I can bore holes on my Haas more accurately than I can measure with my el cheapo micrometers.

[mactec54]

CNCMAN172

If I read it right, You were interpolating a .1574 hole,with a .125 end mill, 1" out of the holder,being 1" out it would flex & is very easy for it to make the hole over size,Unless it was taking very light cuts, A nice carbide .1572 to .1574 reamer would of been better, You could just make some pins to fit the holes, Bore the bearing holes out to the next size bearing, or put a sleave in for the bearings you have

[John Bennett]

MDF is like a sponge and will spring out and come back after the cutter has cut the shape (take a section of MDF and squeeze in a vise). If you cut the MDF with a "small home made CNC" then you have a possible deflection in the spindle, cutter size and the material to consider for fit. That been said, not seen your code, I would plunge a hole (drill) open up to size leaving a few thou for finish cut, and then finish cut. For tighter tolerance,you could leave a little for reaming. Maybe post (or email your code) so we can see how you have programmed this operation)

[tc26]

I did not see anything mentioned about tolerances in this discussion.
When a customer sends me a drawing without tolerances, I tell the boss I'll make the part but the customer may not like it.

[CNCMAN172]

TC26,

We were going for a slip fit not a press fit. The idea was to use the tooling pins to align the parts and use bolts to hold everything securely. We ran numerous experiments and I was shocked I can do a better job on my home made CNC built from Aluminum than we could on a Haas. Just unbelievable.

We did check the dimensions of the paremeter cuts of the various parts and they were right on the money as good as we could measure with a Mitutoyo digital calilper.

I can get the Gcode and post it from the job, have it look on my laptop.

We ran a test where we would drill a hole with a 3/16" drill bit and test a 3/16" tooling pin made of hardened steel. Perfect fit very snug no wobble.

So we ran a test for a 5mm tooling pin which is approximately .197" diameter. We had the Haas drill a 3/16" hole then pause. We tested the hole and the 3/16" tooling pin fit nice. So then we had the program continue and use a brand new very sharp 1/8" 2 Flute carbide endmill to contour that hole to 5mm. This means the cutter would only be shaving a very small amount of material from the sides of the hole. We further only allowed the Haas to step the hole down .015" per pass and used ramping to boot, this would elimate any plugging. The result was a very loose fitting hole we are just completely at a loose for what is happening.

The hole was only going .250 deep and cutting as slow as we were cutting I would have thought it would have been a perfect fit.

We later learned the operator/owner which we watch run the machine had only had the machine for about 8 months and was NOT a machinist with many years of experience. He had taken some training and seemed to know the Haas control pretty well, so he was not totally green.

Regardless the code was processed from ArtCam a program targeted at woodworking industry primarily for designing signs, etc. Don't get me wrong the program seemed very nice. I would have thought the gcode produced would have been pretty standard.

As a second test we had another guy at a local machine shop who uses Mastercam which is known to be one of the higher end packages crank out a small chunk of gcode for doing a tool pin hole and ran than on the Haas and got the same results.

I first thought that the Haas might have been calibrated, but all the corners came out square on the other parts, the dimensions all seemed correct everywhere else, so that kind of ruled out that possible issue. I asked the guy if he had the machine calibrated and trued up by Haas or any certified service center and he said no it only had 300 hours of run time. It did look brand new no question. Anyway, my friend end up spending $1000 for all the machining on the Haas and was pretty disappointed in the final fit, but with lots of work and patience it is much much better than the machine that came from China. We figured he must have got a prototype as some of the machines people are getting from China seem to be pretty true.

Thanks for your comments.

Russ

[John Bennett]

After viewing all attempts to correct this oversize hole. G code I assume is correct but what is not able to be assumed is the size of the cutter or runout. I would predrill and then open up hole with circle mill code and then measure , then compensate for tool size actual. Tool, toolholder and spindle or combination ???? Post your G code and I'll see if anything looks wrong, but I would be looking at tool , even if you measure size with mic, a slight offset can lead to this problem but mic size will show correct.

[CNCMAN172]

John,

Good suggestion, I actually have a digital Mitoyoto mic as well as a digital caliper but the USA carbide endmills measure exactly as advertised when I measured them with my caliper. The Mic would be more accurate but doubt this will yield a signficant difference got to be within .001 worst case.

One thing I did not measure on the Haas was the runout on the spindle. Now I would have expected that to be right on the money probably within .0005 as the bearing are so huge on those things.

My Bosch Wood router runout is probably just under .001 and the bit was .001 under per the manufacturers specs so when I cut it on my home made machine which is built of aluminum I get a very good fit.

I will dig up the G-code file and post it as it would really be nice to find out the root cause. But, with two completely different programs generating Gcode and getting the same kind of results this seems to indicate a machine problem. We might not have been able to measure any significant dimension errors due to a small amount of runout but on a hole with a tight tolerance that might be easier to spot.

Let me look for that code I know I saved the file.


Russ