What is the right - best bit ?????

[Jonboy1955]

What is the best bit to cut 3/4" pine plywood ? Will be cutting out parts for cabinets. Best speeds and feed rates ?

What is the best bit to use for cutting 3/4" PVC???? Best speeds , feeds and depth of cut ????

[Rtalexand]

What CNC Machine are you using? ShopBot Standard or Alpha?

[knight_toolworks]

do you have a vacuum table? if it is smooth you can use a 2f downcut bit. I usually use a 1/4" bit to keep parts in place. two passes one climb almost through one regular through 3ips. 10k a compression bit is really good but it can cause parts to move more.
ref=oh_aui_search_asin_title (https://www.amazon.com/gp/product/B0012K5YDK/ref=oh_aui_search_asin_title?ie=UTF8&psc=1)
https://www.amazon.com/gp/product/B0020B2IB6/ref=oh_aui_search_asin_title?ie=UTF8&psc=1

[garyb]

For the plywood 60-123PLR, 3/8" 2 flute mortise compression, 546ipm 14400 rpm one pass to 3/4"
For the pvc 52-709, 3/8" 2 flute upcut spiral O flute for single pass 250ipm 12500rpm
for 1/4" tooling go to the 63-700 series for the pvc
Gary

[dlcw]

If using a PRSAlpha that is well tuned up, you can use a good quality 2-flute 1/4" compression bit at 5-6IPS/14K RPM. I cut hundreds of sheets of plywood in to cabinet parts every year and always climb cut first, leaving a 1/32" skin, then conventional cut 1/32" thru the material. My first pass is done in 2 passes so as to not flex the machine too much. The purpose of the two-pass system is to help compensate for the flex in the machine. When I use this method the edges are really crisp and right on the money. I can go straight from the CNC to the edgebander. As far as plastic, I haven't done enough to really perfect the process yet.

[Jonboy1955]

What CNC Machine are you using? ShopBot Standard or Alpha?

alpha 4 hp spindle 4' x 8'

[bleeth]

How far are you going with your cabinet parts design?
Line boring for system screws for drawer hardware and also shelf pins is standard at 5mm. For that Centurion tools makes an excellent 5 mm compression bit that can do the whole job for you.
It takes a bit more cutting time for cutting your parts out than a larger bit would but you can process the whole job with no bit changes. or additional machining.

[woodshop]

May I ask, please, what is a "Climb Cut?"
Can that be explained?

We cut maple plywood everyday. Using a 1/4" straight cutter.
We drop down through the plywood 0.125" with each pass running at 60 ipm and 15k speed.
To get through 5/8" plywood, it takes 5 passes.

Thanks in advance.

[garyb]

Its the direction of cut, Climb is clockwise on the outside counterclockwise on the inside, the opposite is conventional cut
Gary

[woodshop]

Thanks, garyb.
Not sure why we would want to use a climb cut, though.
"Google Search Time."

[garyb]

Due to geometry in tooling and the material, the direction of cut makes a big difference on the finish cut.
Old rule of thumb " if the off-cut scrap has a better cut finish than the part, then your cutting the wrong direction"

Here's an example, a mortise compression tool should be ran in a conventional direction for the best part finish, but using say a low helix finisher for the same cut will give the better part finish in a climb direction
Gary

[woodshop]

Really appreciate your explanation. I get it.

Will have to try this.

(Great help, Gary)

[dlcw]

Another thing a climb cut does: because of the bit rotation and feed, the bit is pushed AWAY from the cut line. If you cut all but a tiny "skin" of material on the climb, then reverse the direction of cut to conventional, the bit will be pulled towards the cut line. Because the bit is cutting very little material, the flex in the machine is negligible. This gives you a cut perfectly on the line and VERY clean.

The Shopbots flex. Nothing you can really do about that except minimize it. Either way, there is still flex. This two direction cutting process reduces the effects of the flex to a level acceptable in woodworking. Probably not acceptable in the metal world though.

It takes longer to cut a sheet of plywood but the the end result is much better. I learned this the first time I did a bunch of cabinets. I used only conventional cut with a 3/8" compression bit. Every part needed to have a little edge sanded off. This took a lot of time and manual labor. Back 10 years ago, I was told of this two-pass cutting method. The next set of cabinets I did, the results were ten times better. No sanding. Parts were ready to go the the edgebander without any sanding. Eliminated all the sander labor to create a clean edge on the plywood parts.

[Martin Reid]

May I ask, please, what is a "Climb Cut?"
Can that be explained?

Thanks in advance.

Dear Dave

32433

Those that have used hand routers with a fence will know that machining with the cutter (conventionally) the router and the fence pull together. When on the other hand you machine against the cutter (climb) the cutter tends to pull away from the fence.

So why would you do this?

If you are machining the edges of a quarter sawn timber that has a tendency to spelch or split then although it is difficult to do by hand and down right dangerous on a hand fed wood working machine, climbing against the cutter can prevent spelching.

Also if you are machining around all the edges of a piece then choosing where you start can help to eliminate spelching.

Sincerely and in good faith
Martin Reid

[woodshop]

I really get this and the great explanations offered.

So... You guys are sending two file paths to cut. The first is a "Climb" cut at 1/32" deep.
The second is a "Convential" cut and finishes all the way through the ply.

Are you merging those two cut paths?
If so, how do you ensure the climb cut is first, conventional is second in the Merged file?

[steve_g]

Dave…
Because climb cuts have less propensity to pull out splinters and since conventional cuts are smoother, I cut most of the depth as a climb cut and finish with a conventional cut …

Here’s a typical cut for me in ½” Baltic birch:

First path climb at .225” deep and .010 allowance
Second path climb at .450” deep and .010” allowance
Third path, full depth and on the line… Some of us call this an onion skin cutting strategy.
This toolpath is generated as a single file in Vectric products… under 2D profile toolpaths, edit the passes to three and specify the last to be .050”. Under separate last pass, specify the offset from the line for all passes but the last and check “reverse direction”. I’m assuming you chose climb as the original direction of cut.

If this quick example is confusing, let me know and I’ll be more specific with screen shots!
SG

[knight_toolworks]

another advantage to doing the climb cut is if your bit is getting dull and or the bit jams it will pull away from the part not into it.

[woodshop]

Not confusing here. Good explanation.
I did not know I could edit each pass independently from each other.
Hmm... Onion Skin...Cool!

Yep, will try this ASAP.

Totally understandable, by the way. Great explanations.

Over the past two years, we've been cutting through 5/8" maple 1/4" at a time (5 passes) in conventional mode.

[coryatjohn]

>> Over the past two years, we've been cutting through 5/8" maple 1/4" at a time (5 passes) in conventional mode.

Do you mean 5/4 maple? With 5/8", you've just dug a nice groove in your spoilboard...

[steve_g]

Dave

“We cut maple plywood everyday. Using a 1/4" straight cutter”

I was re-reading posts and just noticed this… Gary Beckwith did recommend a mortice compression bit in one of his earlier posts and I thought more discussion might be in order!

The bit he recommended is a spiral cutting bit. A spiral cutting bit has a cutting edge in contact with the wood at all times, not just when a flute passes by as happens with a straight cutting bit. The spiral bit is a smoother cutting bit because of this feature!

The bit he recommended is a compression bit… that means the bottom of the bit is up cut while the top is down cut. This feature minimizes splintering of the top and bottom veneers by drawing the cutting forces toward the center of the material. The two-flute design he recommended is referred to as 2+2 when you’re shopping… it means 2 up 2 down. I’ve had 1+1 bits in 1/8” diameter and 3+3 in ½” diameter bits.

The term mortice compression means the up-cut portion is very short… maybe even less than ¼”. This allows you to cut shallow rabbets or grooves and still get the benefits of a compression bit! In any case, your first pass must be deeper than the up-cut portion or the top veneer will be pulled up giving a nasty cut!

Spiral cut mortice compression bits aren’t a home depot item… you’ll need to keep a few on hand to assure your supply. The retail woodworking hobby stores may or may not have one in stock… but not at reasonable price! Gary Beckwith reps a quality product in the Onsrud line. Many folks here like https://www.centuriontools.com (https://www.centuriontools.com/). If you live in a metropolitan area, often you can get one or two day delivery from Amazon and most of us have a favorite eBay source.

I hope this little tutorial wasn’t insulting… it certainly wasn’t intended that way! Feel free to ask for clarification on anything I’ve muddied up!

SG

[woodshop]

John: 5/8" maple plywood. 5 passes at 0.125" depth of cut using a 1/4" straight cutter. (Sorry, John... My mistake in an earlier post.)
Steve: Not insulting. We will not be using compression bits. We ordered a bunch of 1/4" straight plunge, 2-flute bits. Our tolerances for the finished cut are not that tight.

Note: We are using VCarvePro 8.5 and when editing passes, we do not find the ability to assign a "CLIMB" or "CONVENTIONAL" direction to each pass. Maybe we need to upgrade to 9.0?

[steve_g]

David…
You choose climb or conventional but then after you choose “do separate last pass” you have the option to make the last pass reverse direction.
SG

http://www.talkshopbot.com/forum/attachment.php?attachmentid=32444&stc=1

[woodshop]

This has been a excellent thread. Great tutorial. Good explanations.

Thanks.

[bleeth]

Taking a 1/8" deep bite is underusing your tool IMHO.
Any cabinet material from Melamine to top quality 3/4" ply can be machined with a 5mm or 1/4" bit in 3 passes on your machine consistantly.
That's why everyone was suggesting a mortise compression as those sizes are made for just that kind of strategy.
I cut cabinets for many years (not braggin-just introducing myself) and never cut as shallow as 1/8" for them even when my SB was an early generation PRT with a max cutting speed of 1.5 IPS
In my shop we cut sides on the bot with full hinge, slide, and shelf line boring and dadoed for an inset back. Others do more machining (tops bottoms and stretchers) for self aligning joinery between pieces.
Don't worry about pushing your tool more. I actually cut conservatively compared to some I know.

[woodshop]

Yes, Dave, and thanks.

I need to be conservative wherever it makes sense. That darn shopbot cost $6k.

[coryatjohn]

>> I need to be conservative wherever it makes sense. That darn shopbot cost $6k.

I don't think you need to worry about breaking your machine. Bits, yes. SB, no. Push it and find the limits.

[woodshop]

We like that LAST PASS REVERSE DIRECTION option. Finally figured out to put a value in the ALLOWANCE field to get it to work.
Nice clean cuts!

(Thanks John and Dave for the confidence to push our machine to the limits. I guess I'm trying to get a hundred miles out of one bit, ha.)

[steve_g]

Dave…

I understand trying to get 100 miles out of one bit! BUT, your cutting strategy may actually be shorting your bit life!

The cutting depth is how much of the edge of the bit is actually working… the rest of the bit is just evacuating chips. By only cutting 1/8” deep, you’re concentrating more of the actual cutting load on less of the bit.

A good, conservative cutting load is 1X the bit diameter, more aggressive cutting is 2X. As machine time becomes more valuable, this is a good place to save time.

When trying to maximize bit life, adhering to the bit manufacturer’s chip load is essential. The manufacturer knows that what kills bits is heat! The chip load is designed to carry away heat in the chip, keeping the bit surprisingly cool.

Another consideration is chip evacuation… re-cutting chips can cause vibration that gives poor surface finish.

I know you have invested in a stock of ¼” two flute straight bits that you need to use to get your investment back, IMHO you owe it to yourself to buy a compression bit to play with and see if next time you need to invest in bits, if it’s the way you should go. Also, you need to know the true capabilities of your machine… The next job may be more demanding!

SG

[woodshop]

Let's add speed to this conversation... We are cutting through maple plywood at 60 ipm's. That's fast for a 1/4" bit of any kind.
Also, I'm listening to the sound of the bit as it cuts. (We have neighbors)
Straight plunge bits cost $10.
Compression bits cost $45
We cut through 5 sheets of maple plywood per month.
If we are cutting slowly, at least we get paid for it. (I quote all my pricing based on 60 ipm's)
We are gentle with the first and last pass through that tough maple plywood.
We are more aggressive through the middle.
The plywood can have pockets of super-hard wood or glue which can break a bit quickly.
Finally, my chip load is spot on.

But I will purchase a few compression bits with my next Toolstoday order.
Won't hurt to give it a try.

[Brady Watson]

Let's add speed to this conversation... We are cutting through maple plywood at 60 ipm's. That's fast for a 1/4" bit of any kind.
Also, I'm listening to the sound of the bit as it cuts. (We have neighbors)
Straight plunge bits cost $10.
Compression bits cost $45
We cut through 5 sheets of maple plywood per month.
If we are cutting slowly, at least we get paid for it. (I quote all my pricing based on 60 ipm's)
We are gentle with the first and last pass through that tough maple plywood.
We are more aggressive through the middle.
The plywood can have pockets of super-hard wood or glue which can break a bit quickly.
Finally, my chip load is spot on.

But I will purchase a few compression bits with my next Toolstoday order.
Won't hurt to give it a try.

60IPM is certainly NOT fast for a 1/4" cutter on a modern CNC with a spindle. If your concern is breaking bits, upsize it to a 5/16 or 3/8" and plow though it. The lowest common denominator here will be internal radii and your design itself. You CAN'T make any money cutting @ 60IPM in sheet goods, unless you are using 1/16 or 1/8" cutters at that speed with a very convoluted design - like a French curve template.

5 sheets is nothing for a micrograin solid carbide tool. Your tooling is NOT the place to save money. There are guys out there that brag about how cheap they got tools - and the quality of their work looks like it. You can't tell them that though...but if the cheap ones were just as good as the premium tools, how can the premium tool manufacturers stay in business? Right. Tooling makes a HUGE difference. Shop on value and not on price. That $45 compression cutter, provided you have adequate hold down, will plow through in a single pass with superior edge and top/bottom veneer finishes. It could last 20-25 sheets, that's 5 months worth of cutting for you.

A 1/4" cutter screams when it is pushed too hard/fed too much material. A 1/4" cutter screams when it isn't fed enough material. Some 1/4" tools scream no matter what. Bump up to a 3/8" and enjoy the lack of screaming...Plus you'll get better chip extraction with the wider kerf, which will keep the tool cooler and make it last longer. You're 3:1 with a 1/4" tool and 2:1 with a 3/8" tool for material thickness vs kerf width. That 1/4" cutter gets smokin hot that deep - carbide ejects from the tool surface when overheated & that means it's one step closer to the trash.

Chipload is not applicable for 99% of what is being cut on a ShopBot. It is strictly a guideline set by manufacturers to maximize tool life. That is all. Nothing else. It is NOT the ideal feed/speed to run for best cut quality; not the best speed to run up to the ragged edge of your hold down strategy before it fails (EG vacuum) or anything else. Forget chipload. Go for a grassroots approach. Sight, sound, smell. How does it look? How does it sound? Do you smell burning? All of these things are on YOU the operator and by becoming intimately familiar with tuning the machine settings, you become better & most confident.

You can start out @ 60IPM as your baseline...then feather in more speed. Keep pushing until you break a bit, break hold down or you don't have any more RPM left to cut a clean edge. Then back it down 15%. There's your feed/speed. These are router machines and not milling machines...so your RPM should never be less than 12,000 on almost anything you are routing. Drilling operations are a different story. All spindles sold by SB are only rated to their nameplate hp from 12,000+. Running lower with a load just heats up the windings...

Toolstoday....I've bought from them. It's a good outfit. However, their price on a 3-flute 1/2" Amana cutter I needed with a 3" length of cut was $135. My local Amana dealer sells them for $87. I'd encourage you & everyone else to establish a relationship with your local tooling guy (or several) and stop paying schmucky retail and over-paying for Ebay garbage. Most DON'T know what they are missing with quality tooling. Once you know what you are doing and the reasons tools break, you get to a point where you don't break tools very often - and that means your quality tools last a very long time before they need to be replaced.

[woodshop]

32445

It's difficult to make something like this too fast.
We prefer to cut slower than the big production shops.

[Rtalexand]

This is a terrific thread. Great info. I recently attended the Cabinet Class at ShopBot for the Cabinet Parts Pro software. I had been using 1/4" bits for all my cabinet work. I am semi- retired and have had my ShopBot for a couple of years and am just a hobbyist, but enjoy building cabinets for myself and friends. In the class, Ryan was using a 3/8" mortise compression from Onsrud (60-123 MW) to cut cabinet parts from 3/4" MDF in a single pass on the PRS Alpha. I am now using the Onsrud 60-120 MW (single flute for my PRS Standard) and I cut a single pass on 3/4" Maple plywood. Using the chip load calculator and listening to the bit work, I am running 288 IPM @ 15,000 RPM. I get a great cut that I can take straight to the edge bander. I can cut a full sheet of panels with dadoes and rabbets in under 40 minutes. So far I have cut over 6 sheets using these settings with no degradation in the edge quality. The bit is slightly warm to the touch when it is done with a sheet.

I hope you don't mind a hobby user jumping in, but the cabinet class was very enlightening ... Thanks

[woodshop]

Amana Tool® Item #46171

Just ordered 2 of the above compression bits.
We shall try these out, compare the cuts, maybe throw some pictures up as proof.

But will probably stick to my standard 60 ipm.

[Martin Reid]

We like that LAST PASS REVERSE DIRECTION option. Finally figured out to put a value in the ALLOWANCE field to get it to work.
Nice clean cuts!

(Thanks John and Dave for the confidence to push our machine to the limits. I guess I'm trying to get a hundred miles out of one bit, ha.)

Dear Dave

Things have moved on from conventional vs climb; so I feel I could contribute another two penn'oth.

From the days of being an apprentice carpenter using a hand router was always 'slow and steady gets the best results'. Moving away from this stand point has proved to be quite difficult and whenever things go astray it is always the fall back position.

But when not using a hand fed machine other issues become apparent.

(1) Taking small amounts off each pass is only working the 'tip' of the cutter.
(granted the reverse last pass elevates some of this by using the whole cutter for the last pass)
A good stating point is a pass depth about equal to ½ the cutter diameter, with the aim of working towards a pass depth equal to the cutter diameter.

(2) Incorrect feeds and speeds increased the temperature of the cutter and reduce the life.
(Generally in plywood - you should see 'shavings' or 'chips' if you are creating 'dust' you need to reduce the RPM or increate the Feed Speed (or a combination of both).

PLYWOOD

The problem with ‘machining’ plywood is the glue lines. On WBP plywood this resorcinol formaldehyde glue is very strong and durable but is also very hard and can dull the cutters. A strategy to vary the depth of each pass to ensure that different areas of the cutting edge cut against the glue line will increase the life of the cutter.

32446

'trying to get a hundred miles out of one bit'

This is the aim of most especially those that are paying for their own cutters.

So for all the issues taken above if I can increase the depth of each pass and thus reduce the number of passes for each part. In your case to go from 5 passes to 4 should give you 25% more parts per cutter.

Sincerely and in good faith
Martin

[jTr]

In the class, Ryan was using a 3/8" mortise compression from Onsrud (60-123 MW) to cut cabinet parts from 3/4" MDF in a single pass on the PRS Alpha.

I would dearly love to see that - I mistakenly ran a 1/4" bit in one pass through MDF and the result was a horribly jagged cut, like I was attempting to cut a straight line with a jig saw. Turns out my pinion gears were worn, but still - I'm simultaneously freaked out yet intrigued about trying this. Just not confident I've got the finesse to tighten up my machine to handle this aggressive cut. (2012 PRSAlpha 9660 2.2HP spindle)

Do you recall feeds/speeds? I'd love to remove 1/4" bit from cabinet cutting routine - 5mm for hardware holes and pins, 3/8" for dados / rabbets. If I could leave the 3/8" in place for cutouts, it would be nice...

Jeff

[dlcw]

A good compression bit will last about 25 sheets (of plywood, 18 particle board) if your RPM and feed rates are correct. The thing to listen for is a bit that is screaming. A screaming bit is a hungry bit. You need to feed it faster or slow down the RPM. I cut 3/4" maple plywood (Armorcore) at 300ipm in two climb passes and one conventional pass.

For mortises in the plywood I use a 1/4" down spiral bit at 300ipm 14K RPM. When I cut plywood, I don't hear the cutting operation nearly as much as the vacuum hold down motors. If I hear the cutting operation (screaming bit), I know I have to increase the feed rate (preferred action) or decrease the RPM's. I've been considering pushing it to 360ipm because I still get a little chirping (other than corners) when cutting. 60ipm is wasting a bit and causing it to prematurely dull.

To give you an idea of feed rates. When you get done cutting all the parts on a sheet of plywood, the bit should be little more than room temperature when done. If it's hotter than that you are dulling and shortening the life of the bit - A LOT!!. Just make sure the bit is not spinning when you touch it. LOL.....

One other side note, when cutting with a compression bit, make sure you plunge into the workpiece the depth of the upcut part of the cutter before beginning you ramp. The up cutters will splinter the edge of the veneer of the plywood if you don't do this. In VCarve or Aspire, you do this by setting your start cutting depth just a hair deeper than the upcut part of the bit. Than do your ramp to cutting depth. Those upcut flutes are VERY efficient!

[woodshop]

Thanks, Martin. I get it. Thanks.
Yes, finally someone understands the hard glue in plywood thing. That's why I choose to go slow.
Also, one must think of those clamps holding down your piece. Pushing too fast and too much of a bite can give your clamps some stress.

IMHO, we can debate the SLOW vs FAST thing all day.

[steve_g]

Dave…

Now that I see your product, I’m not sure a compression bit is the right one for the job! What I’m seeing are numerous shallow pockets, almost certainly shallower than the up-cut portion of a compression bit.

I’ve never cut stair stepped pockets like this in plywood, so my next comments are just gut feel!

If this were my job here’s how I’d approach it:

First, I’d cut the blank perimeters with a compression bit.
Second, I’d set up 2 or more locating jigs that hold the parts with cams. I’d use multiple jig locations so I can reload one station while the Bot is cutting on another. With a little editing, you can have the program continuously go from station to station … or pause at a neutral location waiting for a keystroke to continue.
Third, I’d cut the peg holes… Cutting the peg holes before the pockets lets the pocket pass shave the tops of the holes that likely have splinters pulled up. Hopefully the peg holes are a bit larger than the bit you use for this process… that way you can spiral cut them without retractions for chip clearance.
Last, cut the contour pockets with a down-cut spiral bit.
Oops, looks like there’s some v carving in there also. Do it any time that works!

I often go to great lengths to minimize or eliminate bit changes but there’s no way to do it on this project, that’s why I cut the blanks first, so the bit changes are done for batches.
I’m curious as to how others might approach this job… let’s hear from ya’all!

SG

[Rtalexand]

The class used the Onsrud Chip Load Chart. For MDF, the Chip Load is .019-.021. As I recall, max speed for the Alpha is 600 IPM. So, using the calculator; setting CL=.02; Speed=600; 2 Flutes; the spindle speed is calculated @ 15,000 RPM. Ryan suggested using the maximum router speed to obtain as much horsepower as possible. Slower speed, less horsepower. For my PRS Standard, I had to drop to a single flute bit since max speed is 300 IPM. Once I used these settings, I started getting really nice chips from the cuts.

Yes, it's really nice to combine the toolpaths for the 3/8" bit to do the straight and blind dadoes on the 3/4" plywood and MDF with the profile cut in one file.

If anyone is interested, my Shopbot (used) came with an Onsrud 60-123 MW 2 flute mortise compression bit that I can't use.

Regards, Rick

[woodshop]

The cribbage board was just an example of some of the things we make here.
The subject of my original questions were all about maple plywood and editing passes.
Thanks

[jTr]

Rick,
Thanks for info. I actually bounced back to Garyb's post on page one. Thought it was crazy, but just ran a sample of MDF at his settings (9.1ips, 14,400 rpm, .375 compression bit). Damn! I had no idea my machine could pull that off! Really shows the finesse of ramping values - swift, but graceful, not the reckless action I was imagining. Guess I've been stuck in newbie chicken mode for years here. This changes everything - thank you all for posting - It's been enlightening!

(I apologize for hijacking, Dave B!)

I love my shopbot!!!

Jeff

[Rtalexand]

Hey Jeff,
I struggled with 1/4" bits for 18 months until I attended the Cabinet Class. I was stunned my standard could profile cut that fast and clean. BTW, Ryan suggested a 4" ramps.