Drilling holes

[wildcat]

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

[wildcat]

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]

Originally Posted by 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

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.

[wildcat]

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.

[wildcat]

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?

[wildcat]

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.