Short

[coach]

what would cause entered dimension to be 1/16" short in the X. The Y dimension is good but the x is almost always off.

[richards]

David,
We might need some more information before answering that question. What version of software are you running? What was the total move distance for the X-axis? What was the total move distance for the Y-axis? What was the move speed? What cutter were you using? What was the cutter's depth?

I often have a 1/16th inch error when I'm doing a deep cut with a 1/4-inch cutter. The last cut that I usually make is to cut away the parts from any left-over material on a 4X8 foot sheet of material. Because I don't really care how accurate that cut is, I just give a command to cut as deep and as fast as the machine can handle. The cutter's flex often means that the cut is out of tolerance (but perfectly acceptable for what I need to do).

[coach]

part wizard 3.5.5
the cut was 70" another was only 16"
ON THE 70", the Y WAS 25" on the 16" Y was 4".
speed was 4" per second. cutter is 1/4" down spiral. Depth is .400 first pass, .780 total.
Actually 1/16" is acceptable except I make many same sized tops so I cut the length of the build up too. I also make a lot of radius tops and would like to make the build up for those also. Would save me many man hours from trimming on the cut off saw or trimming with hand router.
thanks,,,Dave

[richards]

Dave,
It looks to me like what you're getting is about what I would expect with my machine. You might want to try Gabe Pari's cutting method, which is to make the first pass(es) climb cuts, and then making the final pass conventional. I've been using that method since I visited Gabe's shopt more than a year ago, and I have found that my cuts are much more accurate and much smoother than they were using the old method.

[coach]

Thank You Mike. I will try that first thing in the morning.

[knight_toolworks]

also try going slower. what material are you cutting? 4" a second may be pushing a 1/4" bit. well most bits really chip load is pretty high.

[coach]

cutting 3/4" particle board.
Will also try going slower. any suggestion as to what a good travel would be?
also what about rpm? I have 2 h.p. spindle.
thanks,,,,,,,Dave

[knight_toolworks]

particle board is not too bad. at 16000 rpms about 240 ipm if your cutting at the depth your cutting would be the best chipload.

[richards]

Dave,
You'll find a Chipload Calculator in the Tools menu in SB3. For particle board, I usually dial in a chipload of 0.015 to 0.020. With a 2-flute cutter, that gives me an RPM setting of 12,000 with a move speed of 6-ips to 8-ips. Twelve thousand RPM is as low as I like to run my spindle except when I'm drilling. The torque curve shows that I have constant power between 12,000 RPM and 18,000 RPM, so I stay within that window. Many times, I use a 1-flute cutter in order to cut the move times in half. I've found that parts with lots of short moves or small curved surfaces cut better at lower speeds. With those kinds of cuts, the machine often stays in its ramp-speed zone anyway, meaning that faster speeds are never achieved.

What I have learned is that with the kinds of cuts that I normally make, if the cut sounds like paper tearing, then I've got things dialed in pretty close. If the cutter screams and screeches at me, I'm spinning the cutter too fast or I have my feed speed to low. If the cutter sounds rough or is low pitched, I probably running at too low of an RPM or I'm running at too high of a feed speed. Also, different brands and types of cutters have different characteristics. I've found that CMT cutters have a very narrow RPM range on my machine where they sound right and that Whiteside and Onsrud cutters normally tolerate greater variations without squealing at me.

[fleinbach]

David,

Read this post it may give you a better idea of what is happening including one more solution to correct the error.

http://www.talkshopbot.com/forum/show.cgi?tpc=29&post=16165#POST16165

[jhicks]

Frank & Mike, I've reviewed your posts and conclusions and was very interested since we seem to be experiencing the same concern. The problem manifests itself cutting along the x axis meaning the Y dimension on 2 equal shelf panels varies. For some reason this doesn't appear to happen on the X dimension. Maybe 2 motors vs 1 on the X vs Y on my prt ?
I have been cutting 3/4" MDF veneer, 3/4" ply veneer, and 3/4" platform ply veneer, 3/4" melemine. All with 3/8" compression bit 2 passes with .050 allowance/offset in 1st pass .550 deep and 2nd pass clean up to cut full depth the additional 1/4" or so to .780 deep since we need to accomodate different material thickness variations between lots. Best speed seems to be 160IPM with ramped in tool path.
The concern is not the 1/32" undersize per se, but rather one shelf or side panel will be 1/32" under and the one above it on the Y dimension same size will be right on or 1/32" over for a combined error of 1/16".
In some cases I see a visible step on the lower x side of all pieces extending 1/32" or more outside the 1st pass even though we're moving in the .050" for clean up pass.
Tried climb and conventional but the only difference is which side the error is on top vs bottom of the panels.
Parts are vacuum held and not moving.

Is it the considered opinion that this is as good as it gets???
Why would one panel be different than another with the exact same art and cut strategy?
I have calibrated my Y by cutting scribes and brad point drilling on the scribe lines to confirm accuracy on 1" centers up the 60 inches of the y and along the 120 of the x so with low load its dead on.
We confirm and calibrate for square as a daily routine befor any cuts and often inbetween if we experience any bogging down or hiccups of any kind.

I could live with consistently undersized parts off 1/32" to 1/16 although 1/16" is pretty darn off the mark but the variation from one to another on the same sheet is not too desireable.
It is however consistently inconsistent in terms of panels toward the Y48 and smaller than panels toward the Y0.

Any advice??