various SC spiral bits - cutting differences

[Ajcoholic]

Before I purchased my Shopbot Buddy, all I ever used in terms of straight bits in my shop were 1/4" and 1/2" diameter Onsrud up spirals (in both SC and HSS).

Since I got my bot' and since I am cutting a lot of plywood parts, I have been experimenting with cutting in single pass, 2 and three passes - with various model numbers - both in up and downcut.

It is pretty unreal how two or three different bits that seem quite similar (say three downcut spirals with slightly different cutting geometries) can produce such different results.

I am also fooling with how fast I can push a 1/4" bit, to cut 1/2" Baltic birch with an acceptable finish and of course not breaking the bit.

Have any of you guys tried a 1/4" diameter compression bit? I have some 3/8" compression spirals that I have yet to try out, but I havent bought any 1/4" ones yet. Not sure if they would be better or no different in terms of cut quality than a down spiral with an MDF spoilboard.

AJC

[Ajcoholic]

Actually the best "1/4" down cut spiral" bit I have used yet (beats the 2 different Onsrud ones I have tried so far) are from a Canadian tool maker located in Toronto - BC Saw & Tool. Its one that they grind themselves.

I just bought two 1/4" compression bits a few minutes ago on line - curiosity got the best of me. Will see how they compare.

With a down cut, the top is perfect, and the bottom side which is against the mdf spoilboard, is pretty good - just some fuzz which comes off when I put the plywood through the wide belt sander.

AJC

[Ajcoholic]

By the way, I am running at 18,000 rpm and cutting at 180 inches per minute.

I am used to running small bits at a high rpm based on my experience. I see some shopbotters cutting at a much lower rpm, what is the advantage if any? Even 18K seems slow to me... I mean I run 5 or 6" diameter shaper cutters at 6K to 8K... a 1/4" diameter bit at 18K rpm is still pretty slow :)

AJC

[bruce_taylor]

I found that the 1/4 bits showed some deflection when I used them in the past, I use 3/8 compression onsrud 60-121 or 60-123 most of the time and I get good results. I cut a fair amount of 3/4 ply but not as much as some here. I have enjoyed the many projects you are bringing to the forum makes me want to make some stuff I've been putting of a while.

[Ajcoholic]

I found that the 1/4 bits showed some deflection when I used them in the past, I use 3/8 compression onsrud 60-121 or 60-123 most of the time and I get good results. I cut a fair amount of 3/4 ply but not as much as some here. I have enjoyed the many projects you are bringing to the forum makes me want to make some stuff I've been putting of a while.

Bruce,I think I hit the max feed speed with my 1/4" bits as if I cut any faster, the interior cuts are undersize. Would make sense...

I bought four 3/8 Onsrud bits (two compression, two down cut) but I am still waiting for my 3/8 ER25 collets. I had ordered one and they sent the wrong size... should be in any day. I think the 3/8 will be the winner - as I should be able to cut faster, in one pass and still hold an acceptable edge finish quality. Yet still not "waste" too much material.

I am quite thrilled to think my simple projects are "inspiring" to anyone... :)

AJC

[bruce_taylor]

I cut 2.5 ips and 11k rpm and make 2 passes. I slowed down my rpm a while back after reading a post about chips vs dust and found my tooling lasts alot longer and I started getting chips instead of dust. Can't remember who or much else about it but it helped me. I suppose you could do one pass but I don't. I don't have nearly the time I once did to play with little projects with my kids being a little older and so many other commitments going on all the time. So anytime anyone makes most anything with a cnc it inspires me and reminds me of such a cool tool that once you have for a while can be taken for granted a little I think. So keep up the good work your a nice addition to the shopbot community!!

[Ajcoholic]

Bruce,
I will try a slower rpm - although it is hard to tell on plywood if chips are being made (the dust is very coarse, so I know its not "dust" as such) but I am also willing to try a slower spindle speed. You never know until you try.

AJC

[knight_toolworks]

I cut most things like mdf and plywood at 3ips and 8k. passes depend on the material. I pretty much always use two passes a climb cut almost through (this is one or two passes depending on the hardness of the plywood) and the second or 3rd pass is a regular cut all the way through. this takes care of the slop in the machine. 3/4" mdf two passes 3/4" plywood (not baltic birch) two passes.

[pkirby]

I cut most things like mdf and plywood at 3ips and 8k. passes depend on the material. I pretty much always use two passes a climb cut almost through (this is one or two passes depending on the hardness of the plywood) and the second or 3rd pass is a regular cut all the way through. this takes care of the slop in the machine. 3/4" mdf two passes 3/4" plywood (not baltic birch) two passes.

Andrew,
I want to emphasis the importance of Steve's statement. I struggled for weeks on getting a nice edge finish. It wasn't until a camp at Gary's place that I learned this secret for the perfect edge finish. Here's some further explanation:
When you make a pass in "climb" the deflection of the bit will go to the waste side of the part. In other words, your part will be slightly oversized. So I typically make my climb pass the thickness of the part minus 0.035". Then I make a second pass in conventional that goes all the way through. This pass trims up the rougher one to a perfect size and finish.

In regards to RPM and chipload, here's a helpful chart
http://www.vortextool.com/images/chipLoadChart.pdf

PS. Onsrud also has some valuable charts and information in their printed catalog.

[knight_toolworks]

except aluminum that needs a climb cut. and single direction bamboo god I have to cut that only with a climb cut and I need smooth edges it takes three passes in 1/2" to get it really smooth.

[knight_toolworks]

Andrew,
I want to emphasis the importance of Steve's statement. I struggled for weeks on getting a nice edge finish. It wasn't until a camp at Gary's place that I learned this secret for the perfect edge finish. Here's some further explanation:
When you make a pass in "climb" the deflection of the bit will go to the waste side of the part. In other words, your part will be slightly oversized. So I typically make my climb pass the thickness of the part minus 0.035". Then I make a second pass in conventional that goes all the way through. This pass trims up the rougher one to a perfect size and finish.

In regards to RPM and chipload, here's a helpful chart
http://www.vortextool.com/images/chipLoadChart.pdf

PS. Onsrud also has some valuable charts and information in their printed catalog.
thats a much better post then what I think thanks for the clarification.

[shoeshine]

Hey Steve,

I actualy have a student here in my new shop that wants to do a whole lot of plyboo cabinetry. Any chance of some further info on bit selection, speed/feed, and cutting strategy? I've never worked with the material and I don't have any good references to point him torward. the stuff is expensive enough that we don't want to do too much (some of course, is inevitable) test cutting for the first run. A general starting point would be most welcome.

Thanks
Chris

[gene]

I cut 3/4 plywood 13000 rpm at 5 to 6 ips full depth with a compression cutter

[knight_toolworks]

Hey Steve,

I actualy have a student here in my new shop that wants to do a whole lot of plyboo cabinetry. Any chance of some further info on bit selection, speed/feed, and cutting strategy? I've never worked with the material and I don't have any good references to point him torward. the stuff is expensive enough that we don't want to do too much (some of course, is inevitable) test cutting for the first run. A general starting point would be most welcome.

Thanks
Chris
I still use the 3ips and 8k for it with three passes 3/4). two to cut through ( and a cleanup pass. the cleanup is critical in bamboo as you get a lot of ripples in the cut from the endgrain in the middle. the bigger the bit the better as bamboo really causes bit flex.

[jTr]

Newbie needs clarification:
Are you plotting two toolpaths per vector to get the two distinct cuts for the climb cut followed by conventional, finish cut, or is there a more streamlined method in partworks?:confused:

[adrianm]

It's done with two toolpaths but if you use Toolpath templates it's really quick and easy to do.

[Ajcoholic]

Well, I tried Steve's method today (one pass 10mm deep climb cutting- and a second pass 13mm deep conventional) with the 12mm Baltic.

Wow! - it gave me a PERFECT finish, and the interior dimensions are BANG ON. :) Also, the bottom had nearly no fuzz, and no tearing out.

I always say, nomatter how long you work in this industry there is ALWAYS something to learn...

Thanks guys - I really appreciate the feedback. I still am wanting to try the compression bits, but I know now that even with a down cut spiral a near perfect finish is possible.

Thanks Mr Knight!

[sailfl]

I have had some good success with Centurion Tools Motise Compression Bits.
1/4" Mortise Compression 1" Cut Length
SKU: 14CR21.02.5FEM200 (http://centuriontools.com/router_bits_toolcase/centurion_tools_showcase.html?page=full&cart=133348924810494919&__max=6&--eqskudatarq=14CR21.02.5FEM200&id1=374&id2=6&id3=734)

But I think I will try different directions and see how that works.

[chiloquinruss]

In past threads about feeds and such I learned about where the heat goes when cutting. If you leave the heat where the bit is (too slow speed / to fast a feed), it eats the bits. When you are cutting the chips should be warm and when done the bit should be warm to the touch - not hot! With my scale buildings I cut a lot of plywood and all of it junk ply from HD. If I don't check each sheet I get into trouble and the bits just go away very quickly. Every sheet is slightly different. Another reference I noticed was the folks doing plastic work and read their threads about melting etc,. It was all about speeds and feeds. The only plastic I cut is sentra and I just use the same settings as I would for the same size of ply if that makes sense? Most junk ply I cut at 13 to 15 K and 130 to 170 feeds. 1/4 inch downcut spiral mostly with some detail stuff with 1/8 ball or 1/16th tapered. I have a 48x96 std with a spindle. Russ

[dlcw]

I cut 3/4" prefinished maple plywood (veneer core) with a 3/8" MC bit at 6ips at 13K rpm in 2 passes.

3/4" melamine I cut with 3/8" MC at 5ips at 14K rpm in 2 passes - same as plywood.

1/2" MDF (sign and plaques) I cut with a 1/4" MC bit at 5ips at 10K rpm in 2 passes - same as plywood.

1/4" MDF (plaques) I cut with a .1875" down spiral at 4ips at 9K rpm in single pass.

All my sheet goods I cut in 2 passes. First pass is climb cut (push bit away from the line). Second pass is conventional (pull the bit exactly to the line).

Super crisp edges ready to go straight to the edgebander. No sanding.

[beacon14]

I use 1/4" single flute compression bits from Whiteside. Using the climb/conventional method takes care of any deflection of machine or cutter. I cut the rough pass in one pass (.73" deep) at 13-15K RPM and 5ips. I tried the 2-flute compression bits but I can't push them through the material fast enough to get a good cut. With the single flute bit I get great edge quality and the parts sizes are as close to perfect as I can measure.

[Ajcoholic]

Well, I finally took delivery of my 3/8" collets today. I tried a few parts cut from the 12mm BB ply, using the 3/8" spiral compression bit (Onsrud). Made the "two pass" cut (1st at 10mm deep, climb cut & the 2nd at 13mm conventional cut).

Spindle speed 15K, 180 ipm feed.

I was excited with the quality of the cut from the 1/4 downcut... well DOUBLE WOW! The compression bit left a perfect smooth edge, exact dimensions and not one chip or fuzz left anywhere. I think I've found the perfect bit and method to cut the plywood :)

AJC

Thanks again for the help fellows!

[bruce_taylor]

Impressive when you pull those parts out of the machine and they look like that. Really shows what the machine is capable of, You might try backing down your rpm's a bit, I found I got much longer wear out of slower rpm's.

[Ajcoholic]

Impressive when you pull those parts out of the machine and they look like that. Really shows what the machine is capable of, You might try backing down your rpm's a bit, I found I got much longer wear out of slower rpm's.

Ill try going down another 2K rpm and see how it is.

I might also try and speed up the feed, but its pretty quick as it is.

ALso, now that I am doing two passes, I am not using tabs which is nice, since the part is ready right off the machine.

AJC

[Ajcoholic]

Well, I just looked at one company's recommended data list and for a 1/4" double flute spiral, at a feed rate of 3 ips (180 ipm) they recommend a 10,000 rpm spindle speed!

I will have to try turning down the rpm or feeding faster (or both).

AJC

[Ajcoholic]

Well, I have cut up at least 5 to 6 sheets of 48"x96" material now, using a 13,000 to 15,000 rpm and a feed speed of 180 ipm.

Even at 13,000 the cut is near perfect, and the bit isnt even warm after several hours of cutting.

This method works really well. Thanks again guys!

AJC

[jTr]

Andrew-
This thread has been a great ed in bit selection - Using Vortex chip load chart, I've been on a different side of scale and have experienced improved cuts. For example: 3/8 2 flute downcut spiral 300ipm / 8-9,000 rpm.
Sounds a little coarse in cutting, but results are awfully good - may try increasing rpm. Chips are upwards of 3mm length, bit never exceeds room temp. Honestly the best cuts I've experienced so far, but there's always room for improvement...

jeff

[Ajcoholic]

Andrew-
This thread has been a great ed in bit selection - Using Vortex chip load chart, I've been on a different side of scale and have experienced improved cuts. For example: 3/8 2 flute downcut spiral 300ipm / 8-9,000 rpm.
Sounds a little coarse in cutting, but results are awfully good - may try increasing rpm. Chips are upwards of 3mm length, bit never exceeds room temp. Honestly the best cuts I've experienced so far, but there's always room for improvement...

jeff

Jeff,
I am a little "scared" to push the 1/4 spirals past 200 ipm... I know at that speed (and 13,000 rpm) the cut is great, and the bit is not heating up. I dont want to snap em' off :)

I have several 3/8" spirals I have bought and will try to run them faster, like you are.

I have learned a lot in the past month, trying various feed speeds, climb and conv. cutting, and different depths of cut. a LOT... and they say you cant teach an old dog new tricks! Bow wow!!

AJC

[jTr]

Of Note: 3/8" bit, climb cut 60% through material, finishing with final conventional pass was absolutely astonishing quality - no witness lines or chatter. On final pass, you can actually see the bit shaving that last 1/64" of material, bringing part down to final dimension. (isn't a shopbot a woodworker's best friend?)

I agree with your sentiments on those 1/4" bits - I've not had the courage to exceed 240ipm. Perhaps we should invest in pooper scoopers before we try....!

jeff