Bit deflection ammount

[michael_schwartz]

Would it be unreasonable to assume a 1/8" tapered ball mill could deflect approximately 1/10" away from the cut line while in a climb cut. This would be with a roughing path, but cutting somewhat on the aggressive side in white oak. I forget the OAL of the bit, but it is the Onsrud tapered ball mill that came with the starter set.

The reason I am asking this is that I am trying to audit/fine tune some parts i cut before I run a whole batch. Bit deflection is the only thing I can think of to explain the this particular error beyond the usual machine slop which is normally well within .01"

I am planning to change my tool paths to fix this, but I am wondering if this particular bit could deflect that much without breaking or if I need to look elsewhere to figure this out.

[Gary Campbell]

Michael...
Yes its possible, but how about some more info?

You say climb cut. Did the path go outside the cutline or inside?
Was the deflection in the X or Y travel direction or both?
You say aggressive, what were the feeds and pass depth? Stepover %?
You say roughing pass, why not an endmill for rough cut? BN EM is a finish tool.
What model machine are you running, and when was the last time all the motion adjustments were checked?

[michael_schwartz]

Michael...
Yes its possible, but how about some more info?

You say climb cut. Did the path go outside the cutline or inside?

The deflection was away from the cut line (inside, or on the waste side)

Was the deflection in the X or Y travel direction or both?

This particular part of the cut had the bit traveling along the X axis with the deflection perpendicular to the line of cut. This particular part of the cut would have been cutting into end grain of white oak.

You say aggressive, what were the feeds and pass depth? Stepover %?

5 IPS (XY), 3 IPS (Z) with a 10% Step over. I doubt it made it anywhere near 5 IPS on this particular cut as the length of the cut was just over .5"

You say roughing pass, why not an end mill for rough cut? BN EM is a finish tool.

To clarify roughing pass was done with a .25 end mill, and the region in question had a .1 allowance. I normally set it as .04 (default) so that may be part of the problem.

What model machine are you running, and when was the last time all the motion adjustments were checked?

Standard purchased at the end of 2009. (Has the new style control box) I went through everything a couple of projects ago and tightened the x, and y motor plates. Everything else I have been cutting seems to be ok, and I haven't seen any other signs of machine slop.



Thanks for the reply.

I think I am going to try reducing the allowance on the roughing pass. I had forgotten I set it so high. I may also try reducing stepover, and feed rate down to about 1.0-1.5 IPS. That wouldn't affect cut time too much as I have this region setup with its own roughing/finish path. I will probably also try a conventional cut vs climb for the finish pass.

These are business card holders, that get cut out with a few cuts on the table saw.

[Gary Campbell]

Michael...
It seems you have solved your problem. :D Try your last listed settings and post again if they dont work.

[michael_schwartz]

I will cut a few and see if that fixes it. I have a new bit on order as well as the one I have been using has upwards of 20 hours or so on it.

I was kind of baffled when I measured a compounded error of almost two tenths of an inch between the two cuts. I spent quite a bit of time pouring over the geometry, etc... in Aspire to make sure that wasn't off and everything else I have been cutting has been fine.

I have encountered the effects of bit deflection many times but the side effect is usually only a few hundredths of an inch.

[paul_z]

Michael,

0.1" deflection is a lot. A carbide bit would not survive that kind of bending so it has to be a combination of things. I suggest that you use a massive bit (like a 0.5" end mill) and see if you can move it by applying force to the tip of the bit. A dial guage would be usfull in measuring the deflection but a helper with dial calipers can do just as well.

The machine has to be powered up and at a stop. Be absolutely certain that the router or spindle can not start. Even then, use a piece of wood to put force on the bit in both the + and - X and + and - Y direction. Measure the deflection with and without the force applied. Don't exceed about 20 lb force. It is possible that you are getting significant wear on the pinion gears or rack. The router or spindle might be a bit loose. Your rollers might be a bit off.

You mentioned that you were using a tapered ball bit. Did you account for the taper?

If you can't find the cause, it might be the time for me to visit and maybe we can track it down together.

Paul Z

[harryball]

Related to the thread. I take what I really cut (i.e. a plywood square) and using the same tool path cut a peice of that 1/4" foam from the box store. I then take measurements. Any variation is from the machine and/or bit. If I find the foam part is also the wrong size/shape it is either the tool path or a hard machine problem. It helps me know what I'm looking for and it keeps everything quiet enough I may hear a problem or see a vibration I otherwise would have missed.


/RB

[michael_schwartz]

Turns out the .1 error was my mistake since I was looking at the wrong geometry. When you put a project aside for a month its easy to look at the wrong version of a file.

There was still deflection when I compared the actual parts to the correct file. However the numbers were in the range of hundredths of an inch. I switched to a conventional cut for the finish pass. Its hard to tell what the tolerances are for the batch I ran yesterday since I applied a smoothing filter to the model. I can tell that they are within what is acceptable for what i need as long as NASA doesn't measure them.

I like the solution with cutting the foam as Rball suggested. I will try that sometime. That certainly would have pointed me in the right direction.