Tweaking advice

[chunkstyle]

Hello all.

I cut out some simple counter tops with my bot and noticed a few things that I thought I would ask for feedback.
I was cutting particle board on my PRS standard 4x8 with 2.2 spindle.
I used a .25" s flute down spiral with a pass depth of .30" Speed was 2.5 at 11500 RPM's. That combination made the bit's whine go away.
The shapes of the counters had 2" radius on the inside and outside corners. I went ahead and drew the build up underside pieces and cut them out too.
Normally I would get the top's of the counters cut out and sticj peices of 4" wide strips of the same material to the underside to get my 1.5" counter thickness. Hog off any extra material at the corners and clean it up with a bearing bit.
I thought,"what the heck, let's cut the build up out on the bot and see how accurate it is cutting". So I cut them out using the same outside edge contour and making the pieces 4" wide.
The build up pieces were spot on! The overall dimension on the length and width of the counter top shapes were 1/32" over sized, however. The tool paths were done in the conventional direction. Even the build up pieces were 1/32" over. Can I assume that this is a result of the tool pathing being done in a conventional direction? Even at .30" depth pass?
The second thing I noticed was that the spoilboard had been "bitten" into at different depths and, in one area of my table, not at all.
The spoil board is .5" uldf glued down to a 5 zone plenum plumbed back to a manifold.
I read from previous posts that drawing air and humidity thru the spoilboard will cause it to swell unevenly and may explain why the perimetr of the spoilboard has the deepest tool path "bites". I'm a little stumped as to why I have an area that had no cuts in it. The table was re surfaced about 10 days before this job was ran.
I'm trying to get familiar with all the levers and knobs and thought some advice might speed up the learning curve for me.
Thanks for any advice, it's appreciated.

Tim

[chunkstyle]

Errrrr.....

I just realized that I probably zeroed the bit out at a high spod in my swollen ULDF spoilboard and that is probably why there was a spot in the table (being the lowest) that didn't get bit. Has this been anyone else's experience?
I have been scratching my rear over that for about four days now! I don't know why the light bulb would finally go off after posting the question. Figures...

Tim

[Gary Campbell]

Tim...
My random thoughts, almost following your order of posting....

A downspiral bit "pushes" itself away from the cut line. Packs material in kerf... and has the most deflection of all our bits... use only for shallow cutting when neccessary. If you wish to cut 3/4" material, use a 3/8 compression, if cutting dados use a 3/8 mortise compression. I would expect 1/32 undersize with a 3/8 compression at 6-8 ips full depth. Use a 2 pass, climb/conventional onioinskin combo for extremely accurate parts.

There are a number of factors that contribute to uneven spoilboard "tracks"

Changes in thickness due to humidity change
Airflow thru spoilboard dries (shrinks) center sections more than edges
ULDF compresses with vacuum
Spoilboard may warp up with humidity change. When surfacing, vacuum cannot pull down warp. When a sheet is on top of spoilboard is "sucked down" much tighter than when surfacing.

Is every possible area of contact between spoilboard and plenum glued?

I have seen .050 difference in "bite" on a fresh spoilboard after 3-4 hours of cutting (S. FL) When doing high end stuff we often would cut 10 sheets and resurface, then do another 10 etc.

[chunkstyle]

Thanks Gary,

When you say to use a 3/8 compression spiral what do you mean by 1/32" undersized? Does that mean that you make the part a 1//32" larger than it's final dimension and get finished dimension with the final, conventional tool pass?

I believe I read somewhere that in order for you to get good results you had to make a first pass depth deeper than the length of the up shear flutes at the end of the tool bit to eliminate any tear out. Since I only have a standard there's got to be a limit for how much depth I should go for a 1st pass depth and still be able to move the bit along fast enuff to keep it cool? Perhaps no more than .375"? If that is the case I suppose that the up shear length of the compression spiral will have to be as short as possible?
Sorry for all the novice questions. I didn't realize that the down spiral was the most "sloppy" of the bit's for my intended cutting. I will get an order in for some 3/8" collets and start investigating the 3/8" compression spirals.

That's quite an eye opener about spoilboard dynamics. I will keep your observations in mind for when I have to resurface. I used a paint roller and titebond 3 was applied to my plenum. Me and a helper worked either end of the table to get it on quick and we were very thorough about coverage. I layed down the .5" ULDF, covered it with a piece of plastic paint tarp and ran the vac for apx. 90 minutes with weight on top as well. To bad there wasn't a nice stable porous material for this application.

Thanks again for your time and advice. It's really appreciated,
Tim

[Gary Campbell]

Tim...
No, I was stating that following your cut strategy I would expect my parts to come slightly undersize at the speeds stated. This is an acceptable amount in most shops.

Here is the scoop: if you cut all conventional parts are undersize. Climb... oversize. This is due to lateral forces of the bit when cutting. If you have a larger bit, the bit flexes less. If your machines motion parts are not adjusted properly, you will get more deflection from the machine. The way to tell the difference is to use a square on the edge of the parts. If the bit is flexing, the edge of the part CANNOT be square. It takes both a good eye and a good square to know the difference.

As long as you are not cutting dados shallower than .3, most compressions should work for you. If you are profile cutting parts make your first pass depth equal to your mtl thickness less .035. Cut this pass in the climb direction. This 1st pass will leave an onionskin at the bottom and oversized cut path. Follow this up with a conventional pass cut thru into the spoilboard. This last pass, which is done with little or no load yields the best cutting results, bar none.

The power of the spindle and bit diameter has more to do with max cut depth than your machines speed. Push as fast as you can without losing steps and reduce rpm to gain chipload and cool bit.

Stable porous material? Thats an oxymoron. Very few, if any, materials that are porous will be humidity stable. None of them will be made from wood fibers.

Learn to keep your machines motion adjustments good and snug. Dont rely on a hand push/pull to see if they are "tight". Use a dial indicator with a magnetic base along with a 50# fish hand scale. Put 25-30 pounds of force on each axis and see how much they move.

My guess is that you cant detect .030 movement with your hand/eye unless something "clicks"

[chunkstyle]

Thanks Gary,

Just so I'm not mistaken, are you saying that I should be taking a full depth of material cut minus the onion skin (.035")? This will be cut in the climb and the onion skin is removed, as well as the possible extra material left by bit deflection, by the final pass in the conventional direction?

I had it in my head that a standard prs's shouldn't be cutting that much material away. Not that I remember where I got that idea from. I have been cutting no deeper than .375" with my practice cutting. Perhaps I am confusing don't run a .25" solid carbide bit any deeper than .375/pass?

No matter, if I have understood you correctly I'll start cutting my plywood and mdf parts using your suggestions.

I'll have to rummage around for the scale to check my axis's for slop. Thanks for the maintenance suggestion. I will make that part of a routine along with checking the spindle for plumb. I'm wondering how good I managed to plumb my spindle after thinking about what you have mentioned earlier regarding the thickness variation that will occur in the spoilboard. I used a trammel and dial indicator in the spindle with a peice of .5" float glass on the table but iff the table's spoilboard was wonky..... I'm thinking that it may be best to resurface the spoilboard right before checking the spindle for plumb.

Once again, thanks for the help.

Tim

[Gary Campbell]

Tim...
In order..
Yes
Many SB Link cutters use that same strategy with a 1/4" bit. Maybe some with a 5mm
Experiment. Your spindle rpms and move speed can both be changed on the fly...you will find the right combo for your machine.

[bleeth]

My solution for this issue is similar to Gary's but I do use all conventional. I use 1 bit, the 5mm compression from Centurian Tools, for all cabinet parts. Cutting the parts out is a 3 pass operation with 2 passes leaving an onionsikin and an allowance so the amount being cut on the last pass is so minimal that deflection is also minimal.

Lately I've been using the same strategy with 1/4" compression for my chase wall frames and plates to maximize yield. The 3/8 bit has been idle. If I used it to cut cab parts, I would have an issue getting all the parts out of one sheet that I do.

There is always plenty of other things to do while the Bot is cutting parts.
There is always more than one way to skin a cat.

Getting ready to cut a large number of Corian Radiused corners and will likely keep the strategy similar but, of course, will use an o-flute.

BTW Gary-you still heading down soon?

[erik_f]

This sounds simple, but I have used bits that are pretty undersized for their rating. I was buying CMT bits from a local vendor and they were undersized by 0.003"...this may not seem like a lot...but that adds up to 0.006" overall. That is 0.006" of free tolerance right there just for not trusting the manufacturer. For production guys like Gary and David compression bits are nice and the way to go...but for cheap bastards like me who's SB only cost them money...I really find I have good with straight bits. Obviously their method is the better method...just throwing out the straight bit route for people working on the cheap. Its kind of my poor mans compression bit.