Consistent Chipload

[Chris Robinson]

Hi,

I'm dulling my bits unnecessarily when making dovetail drawers. The tools that I'm using are a 3/8" comp for outlining and 1/4 dc (set at dia. .249") for male dovetail cuts. Both tools are used for outlining and dados for all other rolling nest files. When cutting the dovetail parts, the speed is greatly reduced so, I'm burning up the bits.

Does the THM have a macro that could keep modify the tool rpm in accordance to the feed speed? So that they remain consistently matched? I would think it could be done based upon spindle load or something? I don't know but dovetail drawers are killing my tool life.

How are others working around this? I could see setting up another set of tools in the control for dovetail drawers that have a reduced spindle speed to account for the slower feeds but I'd be screwed when it the control went to cut a long dado for the bottom with the 1/4" tool.

Any suggestions?

Thanks,
Chris Robinson
The Cabinet Connection
1320 W. Main St.
Wytheville, VA 24382

[Forrest Chapman]

Hi Chris,

I probably cut close to 2000 maple fibercore drawers with 1 dovetail tool and 2 comp. 1/4". The other tools are 3/8" DS and 3/8" comp. outline.

I have cut about the same amount of baltic birch drawers with a different set of tools with about the same life. I'm still cutting with both so not sure how many more I'll get.

Call me if you get some time and maybe we can go over your setup.

Forrest

[Chris Robinson]

Forrest,

What are your feeds/rpms for your dovetail tool, 1/4" and 3/8" comp for dovetail drawers?

Thanks,
Chris

[Forrest Chapman]

Hi Chris,

3/8" comp 18000 rpm, 300 ipm plunge and 650 ipm feed. 3/8" Ds 18000 rpm, 400 ipm plunge and 800 ipm feed. 1/4" comp with 1" cutting edge (key for speed) 18000 rpm, 400 ipm plunge and 600 ipm feed. 5/8" dovetail tool 18000 rpm, 400 ipm plunge and 600 ipm feed. This setup is used for 5/8" material and the sequence is 3/8 Ds cut tails down to thickness. 1/4 comp cuts bottom dado and tail outline. 3/8 comp skins outline. Dovetail tool cut sockets. 3/8 comp final cuts outline.

To reiterate again I've been using the same dovetail tool and second 1/4" comp since we were beta testing the drawers.

If you have any problem with this give me a call.
864-226-5256
Forrest

[Chris Robinson]

Forrest,

Thanks for the data. I'm plunging alot slower, 150ipm. The tech that set up the machine had said that was a good plunge rate. I was told that plunging was the hardest on the spindle bearings and I wanted to insure I didn't plunge too fast and damage them. Of course, if you have been running them at this rate for this long, I doubt it's causing undue damage!

Do you use those feedrates/rpms for your standard nesting?

Chris

[Forrest Chapman]

Chris,

For most materials these are the feed rates I use. I did cut 3 units of curved parts out of plywood for some rough framing and ran them at 1200 ipm. It amazed me how clean the cuts were and there was 0 dust left. You should cut as fast as you can without breaking the bit, moving parts or loosing edge quality. When plunging make sure you are ramping slightly, maybe at a 45 degree.

That leads me to something. I'd like to suggest we can choose the ramp angle instead of distances.

Forrest

[Mark Taylor]

Forest...

Does the "Ds" stand for down shear?
Do you use the down shear for cutting dado's in the rest of your cabinet files as well and the comp's for only through cuts?
Thanks
Mark

[Forrest Chapman]

Mark,

Yes, I use the downshear where ever it cuts partialy thru.

Forrest

[Will Williamson]

i see a lot of data from various sources concerning feed and plunge rates used on 4 x 8 sheets of panel products what about solid hardwood lumber specifically, cherry ,white oak red oak . When I was in training class Josh said that he set all feed rate at 1000 IPM so that he could adjust with feedrate percentage knob through the full range of performance 0 thru 1200
I,m not in a position to break cutters to learn feed rates . Recently I purchased one set of nested base cutters in the lower price range and at the same time I purchased another set in the upper price range. The cutters in the upper price range which is basically three flutes as compared to two flutes do appear to produce better quality of cut . Right now though I have a client who has supplied me with a single flute diamond ball cutter to use on his cherry lumber . Forest thanks your imput there are not a lot of experienced machine owners that participate in these forum questions.I appreate the time you spend .So the question of the day is what are the recommended feed rates for a 1/2 " 3 flute compression cutter taking 5/8" depth of cut in cherry and 3/8' 2 flute compression and 1/4' 2 flute compression
Thanks Will Williamson