Cutting BB

[Steven O Smith]

The sales guy's idea behind going deeper into the spoil board was to make sure the downcut part was cutting material. It makes a sort of sense if you don't mind carving up the spoil board that much. Does not sound like the best approach to me.

Your suggested range of cuts is useful. What you are saying is that it doesn't take much downcut to have a clean top edge. I had no idea if the number was 5 mil or 50 mil.

[Jim Becker]

The "optimal" cut quality top and bottom from a compression tool actually does have a bit of the tip into the spoilboard (which is why it's called a spoilboard) as it provides a better "uplift" to avoid tearout on the bottom. That's practical for big machines in production because they typically use vacuum on sheet stock and frequently replace the spoilboard. It's less practical for those of us who are either hobbyists or small operators because the economics are not there for frequent spoilboard changes or milling off so "kissing" the spoilboard has to be good enough. For many materials, that's just fine and the bottom surface should be reasonably good.

[Brian Tymchak]

Not sure I agree with the "deeper into the spoilboard" comment, makes no sense for a compression bit. I use the Bits and Bits version which has a shorter change depth so I just plunge to 1/4". If the UD2101 is close to 1/4", I would setup a test. First I would do 1/4" - 0.005", then 1/4", then 1/4" + 0.005", then 1/4" + 0.010" and maybe a final 0.015". Just be sure NOT to ramp a compression bit. You need to pluge immediately down to the cut depth. From there, I'd chose based on the quality of cut for the top. The bottom cut is irrelevant as the upcut will yield a nice finish. I always zero to the spoilboard for 99% of the jobs I do and I never go more than 0.003" into the board ever.

Interesting. The Jenny compression bits from Cadence Manufacturing have notes in the feed and speeds page to use ramping if possible.

[Jerome Stanek]

I like to use a lead in and ramping to get the best cut

[Jim Becker]

^^ This is effective because the degraded cut while ramping is outside of the cutline/component profile. It's less stressful on the tooling, than a hard plunge followed by immediate acceleration down the cut line. Folks with industrial machines who are using beefier tooling can get away from things that those of us with more modest machines cannot in this respect.

[Michael Burnside]

Interesting. The Jenny compression bits from Cadence Manufacturing have notes in the feed and speeds page to use ramping if possible.

That's dumb. Either an oversight for a compression bit just copy-pasting as you should always ramp a standard endmill, or they meant lead in.

I like to use a lead in and ramping to get the best cut

Lead in and ramping are not the same thing. Maybe you know this already, I'm just saying it here so people know. You can lead-in a compression bit no problem because the lead is happening on the waste side. You cannot ramp because the work-piece side will get tearout by the up-cut until the ramp is lower than the change over. That's just the way it works. Now if your machine has a hard time with 1/4" plunge then I guess you lead in if you have waste to spare, but I'd try to avoid ramping.

I have occasionally used lead-in when I have a bit more waste to give up, but I only do this on 3/8" or 1/2" compression where I'm hogging out 8/4 maple or something like that. I ALWAYS ramp up/down cut bits, usually 2x the diameter of the bit, sometimes 4x if it's something like Bloodwood or phenolic or something really hard.

[Jim Becker]

Lead in and ramping are not the same thing. Maybe you know this already, I'm just saying it here so people know. You can lead-in a compression bit no problem because the lead is happening on the waste side. You cannot ramp because the work-piece side will get tearout by the up-cut until the ramp is lower than the change over.

True that they are different things, but if you do the ramping within the lead-in...by the time you get "to the line", you're at depth for no tearout and have reduced the strain on the tooling to get there.

[Michael Burnside]

True that they are different things, but if you do the ramping within the lead-in...by the time you get "to the line", you're at depth for no tearout and have reduced the strain on the tooling to get there.

No argument here. I can't think if I ever used a lead-in without a ramp honestly.

[Jerome Stanek]

That's dumb. Either an oversight for a compression bit just copy-pasting as you should always ramp a standard endmill, or they meant lead in.
Lead in and ramping are not the same thing. Maybe you know this already, I'm just saying it here so people know. You can lead-in a compression bit no problem because the lead is happening on the waste side. You cannot ramp because the work-piece side will get tearout by the up-cut until the ramp is lower than the change over. That's just the way it works. Now if your machine has a hard time with 1/4" plunge then I guess you lead in if you have waste to spare, but I'd try to avoid ramping.

I have occasionally used lead-in when I have a bit more waste to give up, but I only do this on 3/8" or 1/2" compression where I'm hogging out 8/4 maple or something like that. I ALWAYS ramp up/down cut bits, usually 2x the diameter of the bit, sometimes 4x if it's something like Bloodwood or phenolic or something really hard.

Yes I know that lead in and ramping are different it starts to ramp in on the lead in so I am at the correct depth when it starts cutting the part without the stress of just plunging