this question goes out to all those that have the benefits of a CNC router! until now i have used 1/2 ball nose end mills for profiling cores/sidewall. Im wondering if those who have used these machines for a while have suggestions for something better or am i on the right track?
thanks
Here's what I use: http://www.happymonkeysnowboards.com/MonkeyWiki/Router_Bits
You want to use bits designed for wood, not metal which is what your typical endmill is for.
the current software im using doesn't allow for very creative tool paths, im pretty much stuck to the side to side profiling will the steps left of the core/side wall be an issue thats why i always used a ball nose
Olie,
what type of software are you using?
im using stock shopbot software its a vectric product off the top of my head i cant remember exactly witch version it is. its ok but there has to be better options out there.
its not Aspire, probably vcarve pro
I have also used Partworks3d (shopbots licensed version of the Vectric Cut3d software) for cutting cores. It works ok, not as much tool path control as FeatureCam or other higher end CAM packages but ok none the less. I've played around with several different types if endmills (Onsrud and others) but the one I last used I picked up at Home Depot http://www.homedepot.com/Diablo/h_d1/N-25ecodZ5yc1vZge/R-100660705/h_d2/ProductDisplay?catalogId=10053&langId=-1&keyword=Router&storeId=10051#specifications It is a 1/2" x 5/16" carbide hinge mortising router bit. The down cutting action of the bit prevents the core from lifting and helps keeps the core flat against the vacuum table. This bit cut the bamboo core with the sidewalks attached very cleanly without having the sidewall detach from the core. I think my feedrates were 2.7 ips at 18000 rpm, .1875" roughing pass with 0.050" finish pass (35% step over?) I use either a 1/4" or 1/8" straight 2 flute endmill (make sure it is sharp! I have ones I only cut UHMW with) for cutting the base material.
olie.
ballnose has a very small point of contact for making large relatively flat passes.
i use cheapo bits from HomeDesperate or online for better (carbide).
something more an one inch wide is ideal, i think i have a 1.25, 1.75 and 2.5 in bit set for surfacing.
similar to this, check your local retailer to see what they have available.
I am about to make my first pair of skis since building my CNC, so I've got some unknowns about bits too. I've got a huge selection of end mills, but I don't think those are appropriate.
I got a nice 1.5" bit for core profiling (same one Mike has listed on his Happy Monkey wiki). What I'm more anxious about is sidewall profiling, since that has always been my biggest challenge using the planer.
Should I attach the sidewalls to the core, then profile the core/sidewalls together? Should I profile the sidewalls as a slab (it's a 2" wide slab) then rip it into 4 sidewalls and attach to the core during the layup?
I'm leaning towards profiling the sidewalls separately since I know folks have done that with success, but what bit would be best for that? And maybe more importantly, how should I hold the sidewall down?
My current idea is to use some spray adhesive to glue the sidewall down to some MDF, and then clamp the MDF to the CNC. I'll have to peel it off afterwards, and clean the glue off, but without a vacuum hold-down system I'm worried about the sidewall lifting up when it gets thin.
hot glue dawg
That's all I ever did with the planer (with sidewalls on the core) but even with TONS of hot glue it was always a disaster. Maybe with the CNC the upwards loads on the material won't be as much.
iIll just do SUPER light passes and let it cut for 3 hours
no hot glue to hold down material to cnc instead of spray nasty.
Machine the sidewalls for the difference of your edge step and attach after.
if MDF is sacrificial you can use much stronger adhesive like loctite superglue. I test this method successfully with wood. Didn't try P-tex yet. Also IMHO very important router speed and feed direction
Yep that's the plan. So ok, hot glue it is, and then as far as the bit, same one I'm using for the core? 1-1/2" straight cut? I figure a normal upcut endmill will want to lift it up too much.
Ok I may need some more guidance. Just did some tests with old scraps and didn't have great luck.
Granted this was a 1/2" wide strip, the 2" wide slab may do better.
I hot glued it to some mdf about every 12" or so, with a 2" long healthy bead of hot glue. For tool paths, I'm having it do some roughing passes going side-to-side, but always the same direction so it's convention milling (not climb), and then some finishing passes tracing the profile going tip-to-tail, again conventional milling only.
Taking off 1/4" of thickness with the roughing pass was too much and after a few passes it popped the hot glue off. I changed it to 0.1" depth roughing passes, it seemed to be doing ok but was going to take HOURS to cut so I got impatient. Then I tried seeing how it would do without the roughing, and just going straight to the tip-to-tail profiling. It got one whole pass, second pass it exploded.
So do I just need to be patient and let it cut for hours? I'd guess the total time would have been about 3 hours. I am running at 10,000rpm (slowest my router will go), and 50ipm. I was using a 1/2" 4-flute endmill (up cutting)
As I posted earlier I have a 1-1/2" straight cut router bit on its way, will that work better? Should I do something different for tool paths? I want to make sure I do this right before I ruin a whole slab of sidewall
I would think a higher rpm would cut and not rip.
10,000 sounds pretty high. I have no idea.
2" wide strip is maybe not a good test.
Try a pine plank or fence board.
Perhaps you will be forced to just mill sleds for use in a planer or overhead belt sander.
Iggy still going planer even though they have a cnc right?
10000rpm isn't thaaaat quick eh. especially for a 4 flute. I'd be looking for less flutes I think, just eyeballing your info. Best thing to do is to calculate the chiploading of your bit with regard to feed speed vs RPM. The toolmaker should be able to give you data for the ideal chip loading for a specific tool and material, but if you want a spreadsheet to use as a starting point, drop me your email via pm.
Onsrud's website http://www.plasticrouting.com/ has a lot of info on suggested chiploads for machining a variety of materials. The data is centered around their cutters but you can get a pretty good idea of what loading you should be looking for by comparing your cutter to a similar Onsrud model. I double checked and I cut my bamboo cores with sidewalls attached with epoxy at 3 inches/sec at ~17000 rpm. This put my chipload at 0.005"/tooth which worked out well for the uhmw and the bamboo. Each core took about 15 min to profile. You don't want to cut too slow (small chipload) or you will generate too much heat and the uhmw chips will start re-welding back onto the workpiece. High feed rates and a sharp cutter will put the heat into the chips and carry it away from the workpiece. Best of luck.
Thanks, that is some excellent data for me. What size/style of endmill/bit do you use, and how deep of cuts are you doing?
Also rnordell, how do you hold your cores down when milling? Thanks!
I was running a 1/2 2 flute Amana end mill @ 30ipm @ 18k rpm with .020 stepover and using 3M outdoor double-sided tape because no vacuum hold down. Vacuum hold down is the way to go, and keep the chips off the material or as rnordell says, they'll fuse, though that's not a big deal, just a couple of passes (dry) on the grinder with an 80 grit and they're fine. It's not easy, the heat always makes the plastics warp up off the table, but this should be a good starting point for you.
Thanks dude, I'll give those numbers a try. This will be my first pair using the cnc for everything, making a pair for the wife (!) so if I screw it up, I won't have to deal with it. "no trust me the skis are perfect, it's your skiing that needs repair"
Wait a minute here THIS is your honeymoon? Congratulations man, I hope you guys have a couple of kids with monstrous capabilities
P.S. A vortex cooler would eliminate all the buckling/chips.
you could try building sth like this: http://www.widgetworksunlimited.com/CNC_Pressure_Foot_Clamping_Attachment_p/cnc-pressure.htm
Success!
I got a nice new 1.5" straight flute router bit (per Mike's Monkey Wiki) and profiled two cores, as well as a 2" wide slab of sidewall material.
To hold the sidewall material down I put contact paper on the material, then used spray adhesive to hold it to some MDF, as well as some hot glue on the sides near the tips. It held great, didn't lift at all, the finish came out perfectly smooth and accurate. The contact paper was just so I didn't have spray glue on the sidewall.
I'm going to be doing another pair here soon, and the sidewalls for that pair are already ripped, so for those skis I'll cut the sidecut of the cores and glue on the sidewalls, then try profiling them together. I'll see which method I like best and go from there.
So far so good! CNC rules! I'll get my journal thread started for this year soon.
so glad you finally figured sth out that works for you!
how are you holding down the cores?
For the cores I just had one large piece of bamboo, wide enough for both cores, and a good 10" longer than the cores (roughly). It was just clamped at either end (my router table uses normal machinist clamps), nothing holding it in the middle. I made sure to watch it closely for any lifting, but it did fine.
One boo-boo on one of the cores - as the router was going from the waist of the ski towards the tip, about 6" from the end, some of the bamboo splintered off. I only lost about 3-4mm of width so I can patch that easily.
I was doing conventional milling, so the cutting faces were essentially peeling the wood grain off. I feel like if I do climb milling, it wouldn't have as much tendency to splinter the grain. Any thoughts on that? I'm going to be doing two more cores in a couple of days so I might give that a go.
