X & Y about .020 off

[mudbug765]

Buddy BT32 standard stepper motors.

What should I be looking to adjust? Pockets and holes are about .020 undersize regardless of whether a small hole or large pocket, and exterior profiles are about .020 oversize. How to do I get to the pinion gear under table to see if grub screws need to be tightened? Do I have to pull the powerstick out? Table has a teensy bit of play/slack in it. I can't really tell if Y axis does or not, but since holes are circular, just undersized, then I would guess perhaps Y axis might need tightening too. I heard about tightening eccentric bearing on Y axis but I'm not sure where it is.

In Partworks, I do have the correct bit selected, and no offset that would cause the discrepancy. Older necks and bodies are dead-on, recent production is off.

Should I be looking at cleaning off all the grease from the runners and re-doing lube?

I cut mostly poplar and maple for guitar bodies and necks, also some oak and aspen for some sign work.

Doug H.

[mudbug765]

More info: Router seems plenty tight, using 1/4 dia x 1-1/4 cutting length downcut bits mostly. I have not had a chance to see if shallow, low-stress cuts with a vbit are accurate or if they are also off.

[ken_rychlik]

It makes a big difference if you climb cut or conventional. Depending on the ammount of slop in your machine it could be a few thousandths or major. Also measure your bit with a caliper. Just because it's package tells you it's 1/4 inch does not mean that much.

Kenneth

[dlcw]

Doug,

Kenneth brings up a good point about using a caliper on your bits. I've yet to use a bit in my Shopbot that actually measures what the manufacturer says it is. Most of my 3/8" compression bits are down around .347 not .375. Many of my 1/4" bits are actually around .24 instead of .25. I've got one 1/4" super O single flute bit that measures .218. Measure carefully. As you can see by the bits I use, my cuts would be off by about .01 to .03 if I took the manufacturers word for it. I've cut a lot of plywood and hardwood. Making sure the tool database in Partworks has the correct bit diameters has made a huge difference in the accuracy of my cuts.

In regards to climb versus conventional cuts, when I cut solid stock or plywood greater then 1/4" thick, I will create a tool path that does a climb cut leaving about .0156 material left. I will create a second tool path that follows the exact same line but cut it conventional. The climb cut will push the bit away from the cut line. The conventional cut will cut right on the line because the amount of material being removed is very minimal and shouldn't cause flex in the machine. Both of these tool paths can be saved in the same tool path file so the only thing you notice during cutting is that the machine changes cut direction for the last cut. You don't need to load another file to run.

Good luck.

Don
www.diamondlakewoodworks.com (http://www.diamondlakewoodworks.com)

[Gary Campbell]

Doug...
Kenneth & Don have hit it right on the head. My guess is that you will find that your bit is around .010 undersize. When a high level of accuracy is required, try cutting a slow shallow straight line in hardwood with the bit and use your mic to measure the slot in a couple places. That will tell you what size the bit is.

This is the only way I know of to accurately mic a single flute bit. Some of the compressions are difficult to get edges lined up to mic. Many inexpensive bit sources sell resharpened bits and they are always undersize. They dont always let you know that.
Gary

[bill]

Might I suggest cutting two 2" square pieces and then also two 2" square holes (insde path and outside path). Undersize tooling will cut the square piece large and the square hole will come out small. This will take 4 cuts, a CW square, a CW hole, a CCW square and a CCW hole. The error divided by 2 will tell you how much your tool is undersize. After this, I average the error and re-enter the "new" size in the tool database which corrects for the error. For me it sure saves the $$$ to get tooling resharpened.

[mudbug765]

Very interesting discourse on bit size. I don't understand the conventional and climb cut. Could one of you elaborate? I do appreciate your taking time answer my questions.

you know, I did a profile straight cut on vectors, not optimized. The bit plunged and then when the router moved along the Y axis, the slot was off from where the initial plunge occurred...as if the table shifted over. What I got looked like a j. Similarly, I had set up a straight-line cut along Y that Partworks decided it would cut from one end toward the middle of the table, then cut from the opposite end toward the middle of the table. Of course, where the two cuts met in the middle did not line up. Like the X axis/table has too much slack...need to call SB about how to tighten the table up, because I can push the table back and forth too. I DID notice the bit was a little undersized last week, not the same bit that I cut the good parts with a few months ago. I will pay more attention to that. I may well have resharpened, undersize bits for the price I paid for 1/4 dia 2 flute downspiral bits. Thank you all.

Doug

[Gary Campbell]

Doug...
Climb and conventional are the 2 directions that a cut can be made along a cutting vector. Conventional would be clockwise inside a circle and conventional counterclockwise. The opposite would be true for outside the circle, where conventional is conterclockwise.

Direction affects cut quality in many materials. Aluminum and some plastics benefit from a final pass in climb direction, where most sheetgoods have a much better edge when cut conventional.

I have no familiarity with the Buddy system, so I cannot help you with your adjustments, but your comments leave no doubt that some are needed. Your manual may have some instructions on adjustments. There are also some online on the SB website.

Remember, you may have 2 problems, fix them 1 at a time so that you will know which "fix" will work next time!
Gary

[ken_rychlik]

Gary, you need more coffee. One of those descriptins you gave needs to say climb. lol

Anyway one thought came to mind when you talked about the bigger hole where your tool plunged. You can have the too ramp into the material instead of a straight plunge and this will help that situation a lot.

[mudbug765]

Tightening the pinion set screws, which did move, did not seem to help. There is still movement, but it may just be the backlash in the gearbox.

I adjusted both nuts on the powerstick release rod to make the rack and pinion mesh more completely. This seemed to help a bit.

I also found there was a tremendous amount of sawdust caked on the rear powerstick rollers. I cleaned off all rollers and all rails and reapplied a very very very thin titanium grease to the rails. I could see how this situation might have caused some irregularity in the table movement.

Students are taking exams so I won't be able to run the machine until this afternoon or tomorrow afternoon to find out if it better.

Thanks for the further explanation of climb vs. conventional cut.

Doug

[Gary Campbell]

Kenneth...

Nice catch! Thanks. CLIMB is CCW on the inside of a circle. CW on the outside

[mudbug765]

Telling Partworks the actual size of the bit, 0.2435" has helped tremendously with getting parts more accurately sized...holes are still a little bit oblong, it's slight.

Doug

[ken_rychlik]

Doug, Look at the ramp options on dado's and cut outs. It won't help on a straight hole, but it seems to wiggle less when you ramp the bit down into the work instead of a plunge.

[ken_rychlik]

Doug, Look at the ramp options on dado's and cut outs. It won't help on a straight hole, but it seems to wiggle less when you ramp the bit down into the work instead of a plunge.

[mudbug765]

The truss rod slot in the guitar neck is a straight run, I use a non-optimized profile cut on-the-line, and ramping wasn't an option like for a pocket. That's where it would plunge and run, and bit deflection would result in a j type hook at the beginning of the cut. I'll go in and make my own code to make it ramp, for a simple straight line cut it will only take a few lines. I can get the line numbers for each depth pass from the SB preview. I can live with the circles being slightly off for now.

Thanks for all the help.

Doug

[Gary Campbell]

Doug...
It is my guess that you still have something loose in the Z mechanism. Although possible, it is very unlikely that you can deflect a 1/4" bit with a plunge and short move. Remember... if the bit is deflecting, the side of the part is angled.

When the Z rollers, Y rollers, even the table roller wheels have a small amount of slack in them they can contribute to both crooked and offsize cuts. Keeping the pinions tight against the racks is important also.
Gary

[ken_rychlik]

I agree something has to be loose, but ramping will minimize it. Does part works have Fluting like Vcarve pro does? If so you could do a ramp on a flute and then follow it with a straight cut.

I would power up the machine and start pulling and tugging to see where the slack is.

It took a welding machine to clean mine up. lol

Kenneth

[navigator7]

@ Doug,
I hope I can interject some humor...but a climb cut is like using a table saw backwards! ;-)
On the manual mills I've run....you avoided climb cuts like the plague.
Tool breakage is always a possibility, ejecting the part from it's fixture, and creating scrap is my definition of climb cuts.
Running a hand held router in the wrong direction is a climb cut.
I see no reason to believe the same principles wouldn't apply to any machine operation.