|Home » Forums » CNC » Message||Login|
You are not logged in. Consider these WOODWEB Member advantages:
Live edge tip1/21
Hi all hope your having a great day
I have a wood slab that i need to flatten i have a flat table cnc router
Thank u all
If you set-up a pocket toolpath, use a raster routine. Experiment with a shallow depth cut to see what angle for the toolpath produces the least tearout. I used shims under the high corners to keep the slab stable. If it is heavy enough no holding is required. I set my DOC to .06" and toolpath depth to below the lowest point on the slab then stopped the router when I was satisfied with the surface. Surface bits need a shallow ramp or have it start cut depth outside of the slab.
I've done this a few times. The first time I found that my regular 4" diameter insert fly cutter was too large a tool for the job and would stall the spindle.
The 2nd time I did it I used a 2" cutter and it worked better but was still easy to stall the 10 hp spindle.
The reason this is a problem is that when fly cutting a spoil board you are taking off a relatively consistent few hundredths of an inch. With slabs the surface varies and you can unexpectedly be taking off 1/8" to a 1/4"......which is too much on a large tool even with a 10 hp spindle.
My suggestion is to use a max. 2" dia. cutter with an approx. 50% overlap. Also try to find your high spots more thoroughly than I did in my projects and set your initial tool height accordingly.
When we do large odd shaped slab flattening my routine is to stand above the slab as high as I can get (step ladder if needed) and I take a photo from directly over the slab with a tape measure laying on the slab. I then import the photo into software and scale the photo to the tape measure. I then quickly vector around the shape of the slab and pocket from there.
We run a 5Z insert fly cutter that is just under 4" in diameter and I typically fire up the spindle and manually find the high spots on the slab with the pendant or keyboard jog. If its way off I may manually hog down some of the high spots until Im relatively close to hitting the whole surface and wont be cutting a bunch of air.
Then just setup a pocket tool path with no profile pass, raster, offsetting the vectors outwards by about 2/3 the cutter diameter. Cut depth/feed/speed will vary based on material.
Very little issue with insert tooling and tearout but if it is an issue we will just run a super light final pass. Large cutter running at 9K and a light/slow final pass and we come off pretty much at 120 grit.
I agree with BH. Big cutter from the start and you find a high spot and you'll stall the spindle and either send a servo off line or shove the part. I find though if I just chop the stepover a bit (we usually run 65% on spoil board) and drop the feed Im ok. Having the pendant is nice because I can set it to "feed" and using the jog wheel and my ear if the cutter is moving into a heavy cut I can dial back the feed on the fly. When out the other side I just bring it back up. If in air, dial it up to 200% until its back in the work.
We typically do the same with wedges as needed and I usually just box the slab in with scraps vacuumed down for the first side and vac down the second side or use scraps again if we cant hold it (holes/checks/whatever).
Watch for flying knots and loose chunks.
When we do this we tend to start high - making a pass or two in air is less expensive than damaging material or tool.
This kind of work for us is just based on time unless we quote it stupid high.
Thank u all for this great tips this is the picture of my bit its a 10 cm bit