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

[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

[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.