Why can't I make round holes?

[Acmeaviator]

I am perplexed - I can't seem to cut round holes
I'm making some new clocks that use wheels which are to large to fit into my drill press. I thought drilling accurate holes would be a cinch but so far I'm just getting oblong holes and ovals. I asked about drilling in the regular forum and got some good insight - but no joy. I need straight, perpendicular, perfectly round holes (up to 3/4") through baltic birch ply (also up to 3/4"). I've tried 1/8" and 1/4" spirals and 1/4" straight all with similar elliptical hole results. A number of people have said never put anything other than a router bit in the Bot so I'm nervous about trying to use regular drill bits (especially as the lowest speed on my router equipped BT48 is 10k). I know you guys drill holes all the time -- how??

[Gary Campbell]

Brian...
You would get better responses if you posted a pic of the results. You should also post your cutting speeds as these can also affect cut quality. Also noting if the oval is oriented in the X or Y direction will help diagnose.

Oval holes on circular vectors are a result of deflection. This deflection can be mechanical or the result of pushing a bit to hard.

Assuming an actual circle in PWks, set up a 3/4" test hole that uses a 1 ips speed in x,y and z. select inside, ramp/spiral. An 1/8" bit wont work well in baltic birch. Use a 1/4 spiral up @ 10K rpm and set the pass depth @ .2 If this hole cuts well, you had bit deflection. If not your deflection is a result of the motion adjustments in the machine being too loose.

Check and adjust all of the bearing eccentrics in the X, Y and Z axes. Do the same for the pinion to rack on all 3.

[srwtlc]

A couple of things to check would be....

Is your machine squared properly? Does it cut square?

Are the X and Y unit values (VU) set the same? Does it move the commanded distance in each direction?

Is anything loose that would allow the machine to deflect during directional changes? Pinion set screws loose? If it's a buddy, is the table secure? Is your material held down securely?

How deep are you cutting per pass? Smaller diameter bits will deflect some during a cut if fed too fast or deep per pass.

Make sure your drawing is correct and that the post processor that you're using is the "arc inch" one instead of just "inch" which can give you segmented circles.

[Brady Watson]

Try the peck drilling option in PartWorks under the Drill Toolpath strategy.

-B

[Acmeaviator]

Thanks as always to your great feedback - I will try all of these tomorrow. I was feeding my 1/8" DS at 1.7 IPS and .1 pass into 1/2" baltic...probably way too fast.

[knight_toolworks]

1.7 is way too fast. I cut a lot of jewelry out of appleply with a 5/32" bit I really battle getting accurate cuts. I can't go over 1ips even when only cutting .08 deep. the pockets kept coming out off center. so I reduced the stepover and they are fine.

[tmerrill]

Brian,

If you are using a ramp setting in Partworks it is the Plunge Rate that controls the speed, not the Feed Rate.

See Tony's explaination here:

http://www.vectric.com/forum/viewtop...al+ramp#p45843

Tim

[Nick McCombie]

Brian,
We've been having this problem for a while as well with small holes. With larger holes (around 1 foot + in diameter) we don't have trouble, but with small holes around the same size you are doing we have trouble. We purchased a keyed drill chuck with a 1/2" post to put into the shop bot. We have had great success drilling into aluminum, plastic, and wood. Then using the drilling toolpath and utilizing peck drilling for thick stuff, it works great. Unfortunately I cannot find the link on the internet to the drill, but I'm sure with a little looking you can find it.
Also, I've heard that one problem with the circles being oblong might be the gearing on the motors, and that you will never get a perfect 1/2" circle using a router bit going in a circle. Hope this helps!

[Acmeaviator]

Thanks for the info - last night I threw in the towel on ever getting true holes with the bot without figuring out how to chuck in the actual drill bits. It must be some interaction between the toolpath and the way the bit cuts - I've to pocket cut holes and inner profile holes both with similar poor results. Even on a 1/4" dia hole using a 1/8" cutter I end up with ellipses. Ultimately it's not a huge deal - I've got a manual drill guide that I can use on pieces too big to fit in my drill press and can mark centers with the bot.

[dana_swift]

Brian, I am a bit perplexed. I make 1/4 round holes with an 1/8 bit all the time. How out of round are your holes? What is the X dim vs the Y dim? What was the design dist?

I have also cut quite a few gears and noticed no eccentricity later when the gears are running. So while the drill option should give you round holes, I am curious as to why our experiences seem so different.

My suspicion is you have some backlash in your rack/pinion for either x or y. As backlash would show up as out of round holes. With the drivers engaged can you move the Z car in either x or y? You might check with a dial indicator and see if any motion corresponds to the amount of eccentricity you are seeing in the holes.

How about some pictures of the elliptical holes so we can compare to our results.

I routinely cut 1/4" pockets with a 1/8 bit and then put die cut parts into them with no visible gaps anywhere, and just a nice snug press fit with my fingers to insert the parts into the pockets.

Most likely you will find the problem and eliminate the drill step.