CNC-Machining Curved Parts from Hard Wood
Advice on bit choice, feed speeds, RPMs, and pre-roughing blanks. May 22, 2006
Question
We have a customer that wants us to machine a quantity of African mahogany. Looking for info about feeds, speeds, tooling, milling, etc. We will be using an AXYS table with vacuum hold down.
Forum Responses
(CNC Forum)
From contributor J:
Don't be afraid of African. I run the same as most other hardwood (white oak, genuine mahogany, cherry). I suppose it depends on what you are doing to material. Cutting, shaping, mortising?
From the original questioner:
We are a Corian shop, not a wood shop, so we are pretty green about cutting wood. The pieces will be 1 1/2" thick with 24" arcs for window jambs. They will then be glued up to 7 1/2" thick by customer. There will be 200 pieces or more. Tried a sample with our 2 flute spiral bit, but I don't see that lasting long at all. It was seaming from the beginning at .5" deep pass, 150 ipm.,18000 rpms conventional cut.
From contributor J:
I use .5" diameter 2 flute 15,000rpm 170 ipm but only .25" deep pass. You should be able to push feed to 200ipm depending on your hold down capabilities.
From the original questioner:
So it seems like this may take quite some time to complete? We have pretty good vacuum and would probably hot melt area of finished piece. The sample I ran was about 1/4 of one piece and it took approximately 2 minutes. So we're looking at 15 minutes per piece to put on CNC, cut, take off and remove scrap. That's 4 an hour, 224 pieces, 8 hour day (probably more like 10), 32 a day, 6 or 7 days roughly speaking. Wow - that would cut into the Corian work. Does this sound like a feasible time frame?
From contributor J:
Try a .3" deep pass. That will take you to 5 instead of 6 passes. Run 18,000 spindle speed. Push feed to 225 ipm. Can you program to run two blanks in one cycle?
From the original questioner:
Yes, multiple sets are possible. I had considered that, and space them far enough apart so we could do 3 or 4 at a time, so we could remove and put new back on before cycle starts again and remove last part at beginning of new cycle, if that makes any sense at all.
From contributor T:
Posted by: themechanic 1/10 [ #8 -- Re: Sugg. for machining african mohageny ]
mechanic@hotmial.com
Get a rough cutter 3/4 up spiral, rough cut leaving 1mm of mahogany, 16000RPM 300IPM. You can cut in 1 inch depth steps. If possible, cut the end grain first to avoid tear on corners, then use a finish cutter 1 pass. Climb cutting works better if you want to push for speed. 3/4 tools will leave better finish, and get tools with cut length just enough to cut what you want.
From contributor B:
This is the type of work we do daily. As long as you have a solid hold down system, you should be able to do the following:
1. 1/2" upcut spiral carbide or HSS 2-flute bit.
2. .55" depth of cut for 3 passes climb cutting at 200 to 225 ipm. The third pass will break the part free so be sure you have adequate hold down power.
3. A full depth clean cut pass conventional cutting (the 3 climb passes can be offset 1/32" oversize but I find it is not necessary). Cut at ~300 ipm.
If you are going to accomplish a high production rate, you have to set this up so you can replace cut parts without removing holding fixtures for bottom access to screw mounts, etc. We use a custom vac pod hold down system. This type of quantity might justify making some custom vac fixtures. You will do better with a rotary vane or similar vacuum system versus a regenerative blower through vacuum panel hold down system.
A simple and fast alternative is to not cut all the way through the material and use screws through the waste areas to hold the parts to a particleboard or MDF spoil board. You would then have to either run the over thick parts through a wide belt to sand away the backs and release the parts, or bandsaw them free and flush the edges on a shaper.
From the original questioner:
What brand of bits are you using?
From contributor O:
Just how long are these parts? How much of the 24" radius is cut going into the mahogany part? If these parts are not really long (8' or so), then you could get these things done in half the time by using a bandsaw, fixture and shaper. Do any of you folks still use these tools?
From contributor B:
Cutting curved blanks is our business. Every size and shape. When we brought the CNC router in the shop to replace the bandsaw/shaper procedure, our production went up 25%. You are right in that a CNC router is not the best tool for every job it is capable of doing. In this case, though, it can be a real timesaver while producing superior accuracy.
From contributor J:
We still rely on the equipment that you mentioned before; however, we have found that radius work on the CNC is faster, more accurate, and safer for all employees involved in a project. No one in my shop has lost a finger while running the CNC. I believe that is an important factor you may have overlooked.
From contributor P:
I thought it needless to spend three to six passes on the router. One would do if the blank were pre-trimmed on the band saw. I do not understand the choice of small diameter bits over larger diameter bits for this process. I believe the screaming would lessen and the finish would improve.
I did want to know the size of the part, wood characteristics, and arc size. Those points would determine whether I would have chosen to pre-trim arc before final sizing of the blank.
From the original questioner:
The job is complete and it went very well. We did indeed rough the parts in to .188 extra all the way around and then cut that off in one full depth pass.
