Bit breaking cutting poplar

[cnc_fabricator11]

We are working on a project involving poplar boards and we are having issues with our onsrud 57-910 1/4" downcut bits breaking on multiple occasions. We've talked to onsrud a few times and verified our feeds and speeds according to their chip load calculations and we still are having issues. The last suggestion they had was to purchase a torque wrench to make sure we aren't over-tightening the collet nut but I don't want to spend the money on a torque wrench if it's not necessary. We haven't had this problem with any other material but the poplar, if anyone has suggestions I would really appreciate it.

Feeds and speeds:

18,000 RPM
.75" thick poplar with .25" cutting depth on each pass
3.4 in/sec


Thanks

-P

[knight_toolworks]

the only thing I see is the rpms are high 8k or so is plenty. I usualy cut at 3ips at that depth in tropical woods so poplar should be fine I would think.

[paul_z]

Is it practical to blow out the cut between each pass?

Paul Z

[beacon14]

How long has it been since you replaced your collet? A worn out collet is a common cause of broken bits.

I agree the spindle speed is way too high. I cut solid wood at no more than 12K RPM, often lower.

Also, are you providing any relief in that kerf for the deeper passes? I find I get better results if I cut the first pass or two in two passes each, with an allowance on one pass, so that I'm routing a wider kerf than the bit. Having the bit follow in it's own footsteps leads to a deep kerf where the bit rubs the walls of the kerf the whole time. Between that and the high RPMs, that could be generating a lot of heat, which is the enemy of router bits.

[bleeth]

What model is your machine and spindle?

[knight_toolworks]

Is it practical to blow out the cut between each pass?

Paul Z
no I mean it would save some bit wear but I have never done it. I rely on sawdust to help hold parts in place.

[garyb]

First thing is what is your chip load size? For the 57-910 is should measure .005-.007. That will tell you if your rpm's are too high or not also what is the temp of the bit? at 18k and a downcut I would expect you're overheating the tool.

Since your running at 210ipm your rpm should be around 15500-16500 to obtain the correct chipload at that feedrate.

secondly where is the bit breaking? if its right at the base of the collet then more than likely you have a bad collet.
Gary

[cnc_fabricator11]

Our machine is a PRSAlpha with a Columbo spindle. We replaced the collet every time a bit broke inside of the collet. We ran those feeds and speeds by onsrud and shopbot and they said that they were fine. I guess we'll try reducing the spindle speed and see if that yields different results.


Thanks for your responses,


-P

[jerry_stanek]

Have you tried an upcut or straight cutter

[cnc_fabricator11]

Yes, upcut broke as well.

[knight_toolworks]

sounds like a bad collet then. I don't think I have broekn a 1/4" bit from resistance befroe.

[jerry_stanek]

run a test with a dial indicator to see if it is the collet of could be a bearing going south

[bleeth]

Chuck up your bit and spin it in the air at a slow speed (3-4K). Take somehing like a steel rule and lay one edge against the un machined part of the bit while you are spinning. If it moves at all you have a problem in collett or bearings. Run the "trammel" test for z alignment. Although 18k is too fast it still shouldn't be popping bits at that speed quickly.

[gene]

what type hold down are you using? if there is vibration in the wood this can cause the bits to snap

[cnc_fabricator11]

We are using a vacuum hold down system with additional screw down. It does seem to be the vibration of the material as we have replaced the collet and collet nut multiple times. Would making more passes in a cut reduce some of the vibration that is occurring? It's really strange because the last time we were involved in this type of project with this type of material we didn't have any issues with material vibration. Also, does anyone have other suggestions for holding down boards/lumber in addition to vacuum and screws?


Thanks,

-Patrick

[bleeth]

What's the size of your boards? Have they been surfaced already?
Have you trammeled your z?

[cnc_fabricator11]

The boards have been surfaced 2 sides (top and bottom in relation to the table). The average width is 6.25". This is the first time I've heard of trammeling the Z, could you explain please?


Thanks,

-P

[bleeth]

Okay. One thing I was thinking is that if the boards are not flat then they may be rocking on the table. With that narrow a size your vacuum may not be helping depending on how you have the zones set up on your table and any area within the zone not covered by the board being handled.
Another thing: If you are, for example, cutting through the board in the length direction as you get through the board you may be experiencing enough of a movement in the board to be grabbing the bit much like a board can pinch a tablesaw blade from tension in the board closing the gap as you cut.
You haven't spoken yet of the effect on reducing spindle speed.
As far as trammeling, this is a way to check that the z is properly perpindicular to the table. See the following link:
http://shopbotwiki.com/index.php?title=Z_Axis
The "bent wire" is a poor mans way of making a trammel and will work fine and the dial indicator is the more technical version.
You can bend a piece of 1/4" rod of some kind (aliuminum from big orange or something and that works.
Need more info about what, how you are cutting to get into holdown comments in addition to screws. Maybe it's time to post a screen shot of your toolpath and strategy.
From your last posts I get the impression that the bit is breaking above the spot where it enters the collett. You aren't by chance putting the bit so far in that the collett is grabbing the cutting area, are you?