CNC router bit suggestions

For discussions related to ski/snowboard construction/design methods and techniques.

Moderators: Head Monkey, kelvin, bigKam, skidesmond, chrismp

User avatar
MontuckyMadman
Posts: 2395
Joined: Fri Jun 20, 2008 9:41 pm

Post by MontuckyMadman »

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?
sammer wrote: I'm still a tang on top guy.
User avatar
More
Posts: 112
Joined: Wed Jul 04, 2012 8:16 pm

Post by More »

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.
rnordell
Posts: 50
Joined: Wed Feb 24, 2010 11:16 am
Contact:

Post by rnordell »

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.
twizzstyle
Posts: 2204
Joined: Tue Mar 07, 2006 8:25 pm
Location: Kenmore, Wa USA

Post by twizzstyle »

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?
twizzstyle
Posts: 2204
Joined: Tue Mar 07, 2006 8:25 pm
Location: Kenmore, Wa USA

Post by twizzstyle »

Also rnordell, how do you hold your cores down when milling? Thanks!
User avatar
Brazen
Posts: 841
Joined: Thu Nov 25, 2010 11:26 am
Location: San Bernardino, CA
Contact:

Post by Brazen »

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.
"86% of the time it works 100% of the time".
twizzstyle
Posts: 2204
Joined: Tue Mar 07, 2006 8:25 pm
Location: Kenmore, Wa USA

Post by twizzstyle »

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" :)
User avatar
Brazen
Posts: 841
Joined: Thu Nov 25, 2010 11:26 am
Location: San Bernardino, CA
Contact:

Post by Brazen »

Wait a minute here THIS is your honeymoon? Congratulations man, I hope you guys have a couple of kids with monstrous capabilities :D P.S. A vortex cooler would eliminate all the buckling/chips.
"86% of the time it works 100% of the time".
User avatar
chrismp
Posts: 1443
Joined: Fri Feb 13, 2009 9:00 am
Location: Vienna, Austria

Post by chrismp »

you could try building sth like this: http://www.widgetworksunlimited.com/CNC ... essure.htm
twizzstyle
Posts: 2204
Joined: Tue Mar 07, 2006 8:25 pm
Location: Kenmore, Wa USA

Post by twizzstyle »

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.
User avatar
chrismp
Posts: 1443
Joined: Fri Feb 13, 2009 9:00 am
Location: Vienna, Austria

Post by chrismp »

so glad you finally figured sth out that works for you!
how are you holding down the cores?
twizzstyle
Posts: 2204
Joined: Tue Mar 07, 2006 8:25 pm
Location: Kenmore, Wa USA

Post by twizzstyle »

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.
User avatar
skimann20
Posts: 345
Joined: Wed Feb 27, 2008 8:28 pm
Location: Taxachusets

Post by skimann20 »

I'm digging this one up from 2 years ago. I have a new bottom mold that I'd like to try and i'm going to become a MDF sawdust making facility. Anyone care to give me some info on what their favorite bit is to cut MDF is?

this is the one that monkey suggested:

a thicker one:

I have a 2.5hp router on my cmc but man I couldn't image cutting this fast:
IslandRider
Posts: 80
Joined: Wed Dec 19, 2012 11:00 am
Location: Kelowna BC

Post by IslandRider »

I'm still very new to this whole CNC thing, but I use $5 ebay tools almost exclusively for MDF. Partly because I crash them more than I'd like to, and partly because MDF dulls tools fast. I've tried HSS, and solid carbide higher end stuff, but none of it worked any better than cheapo ebay tools. MDF will cut as fast as your machine can handle, I can run 1/4" straight flutes up to about 200ipm and .25-.375 depth before the machine flexes too much and I lose detail. Clearing dust out of the groove is most important part. Only time I've broken bits with MDF is when the groove packed back in with dust or something in the program wasn't right.

For profiling cores and making molds I use a 32mm bottom clearing bit (ie straight 2 flute carbide), 3d raster in the long axis, fairly shallow .300 or so cut, and as fast as I can drive the machine before it starts skipping around the shop, so 250-300ipm or so, and then override up from there. Ramp plunge moves or plunge slowly to help with burning tools out. The sound it makes while cutting suggests it could be running faster, but the machine isn't rigid enough to take like the 'pro' one in that video. Some day I will put some thought into feeds and speeds, just been winging it for a year or so and getting better. No spindle speed control hooked up, so 18000rpm for everything on a 1.5hp spindle.
skidesmond
Posts: 2337
Joined: Tue Apr 07, 2009 3:26 pm
Location: Western Mass, USA
Contact:

Post by skidesmond »

skimann20 wrote:I'm digging this one up from 2 years ago. I have a new bottom mold that I'd like to try and i'm going to become a MDF sawdust making facility. Anyone care to give me some info on what their favorite bit is to cut MDF is?

this is the one that monkey suggested:

a thicker one:

I have a 2.5hp router on my cmc but man I couldn't image cutting this fast:
I'll look for the brown cloud in the east. :) When I created my mold I used a regular 1/2in straight cutting bit with a bearing. Seems like the fluted bit will work quite well in the cnc. I used a template/router approach, not a cnc.
Post Reply