Need Advice on Feeds and Speeds

[bjwat@comcast.net]

I was just given a job to make 100 items out of 13/16" Hard Maple. Each item is about 5" X 14" in size. I have a 5HP Colombo and I need a few recommendations:

-Bit geometry: Straight or spiral? (Aiming for 1/2" bit)

-Bit stepdown per pass?

-Feedrate & Z-plunge speeds?

-RPM?

What's the most efficient way to avoid unecessary bit wear when plunging into the material the 1st time?

Any help is appreciated!!!

Thanks!
Brady

[kerrazy]

Hey Brady,
First off , I was pleased to se you will be joining Team Canada Camp ShopBot.

I cut maple with a 1/4 " onsrud Up cut spiral bit with a feed rate of 1.25 in./sec and a max depth of .25 per pass. and a plunge rate of .50 with very good results. As far as bit wear the onsrud bit is solid carbide and seems to stand up well for me. I have also had great results with a 1/4" double flute straight bit as well, again solid carbide.

The noise is pretty loud though with the spiral cutter. It seems to whine pretty good.

Dale

[elcruisr]

Brady, I've cut tons (literaly) with a columbo spindle. You have a few considerations concerning bit selection. What sort of edge quality being the most important. Lets say that you need a clean edge and some fuzz is OK on the top edge. Then I'd opt for a 3/8 or 1/2 two flute up spiral. I'd do it two passses with Z at 1.2 / X,Y at 2 to 2.2. RPMs will vary with the bits manufacturer but I also heavily favor Onsrud and would run theirs at around 12,000 to 13,000. Remember that you want to see chips not dust and the bit shouldn't be either "screaming" or "growling". You'll learn what sounds right with some time.

If you need a good clean edge with an absolutly clean upper and lower edge then you need to go with a compression spiral. Onsrud has a special one with the shortest upcut I've found. More downcut means less lifting force on parts. I'd use a single flute or in a pinch a two flute and similar feeds and speeds.

Do ramped entries if your software permits them. This will prevent burning and extend tool life. If you need to use tabs for part holding keep e'm on the long side to prevent spliting.

Try varying between climb and conventional cutting on a piece of scrap from the batch to see which gives the cleanest results. Alot of people like to claim one way or the other is best but experience has shown me that different batches of wood respond differently and need to be tested.

Good luck!!
Eric

[artisan]

Hi Brady...I just finished a set of Maple signs for a hotel here for their conference area and I have to agree with Dale and Eric about the carbide bits. Spend some money on solid carbide bits as "Sharp Bits" makes all the difference in the world....as does a little patience and multiple passes. I too favor Onsrud and Hartlauer. The Hartlauer 52-1600, 1/2 inch (54.00) is my workhorse for wood cut outs.....D

[bjwat@comcast.net]

Thanks guys!
Edge quality is not critical because I need to run an oval 'table top' edge bit around it with a hand router to get my finished edge. On the original piece it looks like the rounded edge back cuts the material about .0625 so it would clean up any ragged edge.

I like the Onsrud bits too...Gotta make sure I'm making a <SouthernAccent> chee-ip </SouthernAccent>


OK so from what I read here go with an upcut spiral with Z1/XY2 speed and .25/.5 stepdown/pass and 12-13,000 RPM depending upon chipload...Right?

-Brady

[gerald_d]

Everything sounds good, but how are you holding the pieces down? An up spiral may be too much for your holding system.

[bjwat@comcast.net]

I have a vacuum jig that I think will work out well...We'll see how it goes...