[kentavv]

Perhaps someone will be able to offer an opinion on the following. I hope the picture is clear enough... This is a corner of a 3.04x3.04x.25" Al plate. An 8x8 grid of 1/8" holes have been drilled (first with a 1/8" spotter and with 1/8" jobber on a .1" peck cycle). After the holes are drilled an 1/8" 2 flute end mill is used to clean out material .125 deep with .0625 z steps. The walls of the tubes should be .04" thick. As you can hopefully see the holes are eccentric to the tubes. I have repeated this process get a consistent error. The outer diameter of the tube is pretty good at .205 +/- .001 so the arcs seem to be cut fine. Measuring the tube wall is between .030 and .44 (should be .040) The inner diameter of the tube is roughly .006 over sized. This actually accounts for quite a bit of the error with a .004 lateral shift remaining. So the bit has wondered to the left on each hole. This is also easy to see by restarting the program and re-drill the holes with the end mill. The end mill shaves .006 off the part of the and the wall thickness where once was too large is now fine (the other side is still too thin though).

Should I be drilling these holes somewhat differently to avoid the deflection of the bit and subsequent hole enlarging? I don't know if I could reasonably use a centering drilling 1/8 end mill to drill out all these .25 deep holes without breaking it. What do you think? I wonder if a drill mill such the following might help?

http://www.use-enco.com/CGI/INSRIT?P...PARTPG=INLMK32

Thanks

[wizard]

The first thing that comes to mind is the drill bits. Assuming the spotting was done properly and your machine repeats correctly, I would have to think that the drill is not sharpened properly and is wandering.

Well that and a few other things that come to mind. Like how far is the bit sticking out of the chuck? What is the bits length and can you use a much shorter one? Do you have room to mount a drill bushing holder in line with the spindle to control the drill bits start?

There are all sorts of things to consider. For example is the drill alway wandering off in the same direction? This could indicate something of use to you. Are you feeding to fast? Are the chips clearing the bit properly?

Dave

[kentavv]

Wizard - The error is very consistent (off the same amount in the same direction - almost parallel to the X-axis actually) and I believe the mill is repeating fine - at least I can hit the holes again and again. The feed was 4.1 ipm and the speed was 2139 rpm. I don't recall exactly but I would guess the bit was sticking out about 2" - these jobber length bits. It was a new Cleveland Twist bit. Looked like the chips were clearing nice. I was pecking at .1 per pass and using coolant.

What's a drill bushing?

No reason to believe that what I was trying to do is unreasonable though?

[lerman]

The key clue is that the holes are always off in the same direction. I have two guesses (not much more than that):

1 -- You are always approaching from the same direction on the X axis and you have significant backlash. If that is the case, you should be able to lock the gibs in X and Y and try doing one hole; testing it with your end mill test.

2 -- Check that the head of the machine is square to the X axis. Also, that the quill motion is parallel to the spindle axis. If they are not, a difference in length between the drill and mill would cause them to enter the stock at different places.

Ken

[Caprirs]

The key clue is that the holes are always off in the same direction. I have two guesses (not much more than that):

1 -- You are always approaching from the same direction on the X axis and you have significant backlash. If that is the case, you should be able to lock the gibs in X and Y and try doing one hole; testing it with your end mill test.

2 -- Check that the head of the machine is square to the X axis. Also, that the quill motion is parallel to the spindle axis. If they are not, a difference in length between the drill and mill would cause them to enter the stock at different places.

Ken

These are excellent points. The difference in tool lengths combined with the head not being perpindicular to the table can give the results you're seeing. If you have an indicator, place it in the spindle and sweep the largest circle possible on the table of the machine. Over a few inches diameter, there should be less than .001" variance.

[kentavv]

All axises have ball screws and I have only measured .002 of backlash in the Z-axis. I have never measured any backlash in the other axises.

The quill does no longer moves but the head does.

I'll check the tram again. Last I checked it did not seem too bad. It always seems difficult to figure out if the measured error is real or a the blocks are out of square or some combination of the two.

[Newby2]

What is the runout of your spindle? Are you using a dirll chuck or a collet to hold your drill? A collet will run much trurer.
Have you tried a screw maching length drill? Or how about a solid carbide SML drill? Bullet the hole with the RPM as fast as you can.
I run a .224 solid carbide at 2950 RPM, .0025 ipr thru A2 tool steel 1.125" deep, no peck with no problems. Worst runout was .0008"
Also is the hole concentric to the OD of the tube?
Steve

[CNC-OVERLOAD]

After reading this thread, I don't feel drill runout has much to do with your problem since it would not be consistently in the same direction. Runout can and probably does account for your hole size but not the positioning. One thing I would check is the program for a different work offset on the different tools. If the two different work offsets were assigned to the different tools and each was set differently for the x axis it could very easily cause this problem.

[kentavv]

The bit was held in an Albrecht integral chuck. The runout is (from memory) .001 6" from the face (will recheck that). I only have jobber length bits but will order a few drill mills and repeat this part. The hole is not concentric to the tube and that is the real problem. A little hole enlargement would be fine but not a displacement. All errors are consistent in amount and direction and were repeated on a second workpiece.

I have tried two programs. The one that generated the large grid was done with a CAM package. No G54, G55, etc were present. I manually checked the position of the drill cycle and the arcs and they were correct. I also wrote a small program from scratch to drill a hole, and then enter from the left side, mill around the hole forming a tube, and then continue to the right. The hand written program actually seemed to have done a little better. Interestingly enough the seed/feed were both 50% higher in hand written program.

All machining of the part was done after finding the origin once. In other words, I first found the origin with an edge finder (with the edge finder in the chuck), then put in the spotting, then the drill bit, and then replaced the chuck with a end mill adapter. The work piece was not removed until after all machining was finished.

Thanks for the suggestions - I have several areas to investigate now.

[HIRAH]

it looks to me like a program error with the endmill. are you milling the id and the od? when you dry run the program(does anyone but myself do this anymore?) are the machine positions corresponding to the print?
it looks like you are trying to pull an arc from more than 90° but less than 180 and the machine doesn't like it. or there might be a discrepeancy between the initial arc start point and the arc itself.what kind of machine is it?

[kentavv]

I verified the points by hand and start/end and drill points are correct. The ID is drilled; the OD is mill. Coming back with the end mill it is easy to see that the mill is running truer than the drill (the end mill shaves off part of the "thick" part of the tube).

Could you explain what you mean by "it looks like you are trying to pull an arc from more than 90° but less than 180?" I am not sure how to answer this.

This is on an Industrial Hobbies mill.

[HIRAH]

I know that a few of our milling machines won't cut correctly more than 90° and less than 180, or more than 180° and less than 360°.
if you had a circle and wanted to start milling at y0 x-(rad), then you could go 180 or 360 with 1 move.
if you wanted to start at 45°, you would have to start x-(45),y(45), then go to 90, then 180, then 270, then 0, then back to the 45.

[BobWarfield]

I missed hearing a conclusion on the tram?

FWIW, I would try to find a way to measure repeatability at 2 different Z heights for the IH mill head. I assume, particularly with a big Albrecht in there, that there is a significant Z difference for the head in the 2 operations?

It would be interesting, for example, to try boring a hole with a center cutting end mill at the two different heights or even a test bar of some kind and find out if there is any shift as the Z is moving.

The head may be trammed, but is the column squared, in other words?

One test would be to put a DTI in the spindle and measure against a vertical reference (cylindrical square, angle plate, or something that's really perpendicular to the table) and see how much the DTI deflects as you move the head up and down.

If this is the issue, the next step is to either correct the problem or perform the two operations with the head moving as little in Z as possible. On the latter, put a screw machine length bit in an end mill holder instead of Albrecht chuck.

Just a few thoughts...

BTW, fascinating looking part, what is it?

Best,

BW

[kentavv]

Ok, I see. If zero degree is along the horizontal axis and on the right side and increase in the counterclockwise direction when viewed from above (all standard IMHO then these were started at 180 for the CAM generated program and 90 for the human generated program. Both were complete in a single full circle G2. Mach3 1.84 is the control software. The OD is pretty consistent...

When you cut outside the limits on the machines that don't like full circles do they not cut all the way or the path oblonged or something else?

I know that a few of our milling machines won't cut correctly more than 90° and less than 180, or more than 180° and less than 360°.

[kentavv]

Bob - I had another problem with this part. After cleaning out the space the mill came back to clean up the holes. The first time I ran this I retracted and tried to come back to -.125. Unfortunately, the mill overshot a little and little diamonds were left between the holes (neat look but not what I really wanted). This lead me to put a height gage on the table and measure against the head at a few different locations. I found there was .0020-.0035 of backlash which has partially been corrected in Mach3. The second run instead of retracting the mill zig-zagged between the holes back to the first hole so I didn't really test if Mach3's backlash corrected the problem but regardless the part turned out better. So, testing with the height gauge (a Fowler - I didn't break the bank on the height gauge front) the head seems pretty good at repeating position over a large range and now most backlash is compensated for. I had used a test indicator previously, zero it on the table, go up a few inches and rapid down to zero. No broken test indicator and the reading was dead on.

You have a very interesting suggestion about making test cuts at different levels... have to think about how to do that at reasonable cost.

I did measure with a test indicator against a 2-4-6 block (got a set after seeing them on your site actually) and please remember these are no-name Enco 2-4-6 blocks so I don't know their true squareness. Anyway, measuring with a test indicator against them along the 6" there is roughly .003 different in both axis (I think I previously wrote the exact values in this thread). Measuring with a dial indicator (not a test indicator) against a square shows no measurable difference in 6". Which measurement is to be trusted? Cylindrical squares are probably the best but they must be made out of gold.

I previously ignored the small tram errors like in the above paragraph simply because my parts are not that thick so a .003 difference over 6" is nothing over 1/2". I never gave much thought to how it might affect relative positions between tools (in this case a drill and a small end mill). Very interesting.

Unrelated to this thread really but perhaps interesting - Another unexpected source of error has come from my vise. I use a Kurt 688 vise and previously really tighten it down on the part. Well, as material is milled away so is the strength. I have actually measured error introduced by deformation caused by the force of the vise. In the worse case while cutting a slot at full depth I had the slot compress and pinch the 1/4 endmill till it broke. Now, I tighten it a lot more gently.

The part is my attempt at a part made in house for lab equipment. I was not involved with it so I don't know the lab but I do know that when built with a 3D printer it did not build properly. Hey, I had a weekend - if I was not doing this I might have been watching TV

In search of precision...

[CountZero]

@wildcat

Just a tip on slot milling, try to plan the cuts so the slot won't be compressed(make it in the y instead of x direction for example).

@BobWarfield

You have an amazing collection of information on your site, wonderful!

[kentavv]

That's a great idea. Difficult for circles but point well taken. It just shows the tricks one picks up with experience. I watched a training video recently and the guy said that he tries to write the programs to make cuts, when possible, right to left (or was it left to right?) so the chips are thrown away from the operator. It would have taken me years of being beat with hot chips to realize that And that stuff (illusive common sense), doesn't seem to be taught much. I picked up a book recently "Machine Shop Trade Secrets" by Harvey that is full of stuff like this.

@wildcat
Just a tip on slot milling, try to plan the cuts so the slot won't be compressed(make it in the y instead of x direction for example).

[BobWarfield]

Wildcat, you are going to learn it all in the best possible way--through experience!

It sounds like things are not quite square as you move up and down in Z based on the measurements you are getting. Your next question will be whether you want to try to minimize z movements by using shorter tooling for drilling (just to get the job done), or whether you want to start shimming your column until things get really square for the Z moves (a more permanent solution).

I love that you worked on this part even though it wasn't really a "pride and joy" project. Chalk it up as valuable experimentation and learning. I try to set aside a little of my time just to go out in the shop and try things. I usually learn more at those times than when I am on a project. With the project, if something measures out wrong, I just fudge it and push on in order to get done. With experiments, there is no point in fudging it because you are there to learn.

CountZero, thank you for your kind words!

Best,

BW

[ctate2000]

Not a drilling problem. You have a interpolation issue. Check your code for math errors. Check x axis for backlash. Check roundness of OD. Place indicator in spindle locate center of hole then indicate OD and check for out of round condition. The consistancy of the error is indicative of the too problems I suggest you check for.