Cutting Hard Maple with Onsrud 57-910

[Steve Wonser]

I am a newbie with regard to the ShopBot. I purchased a Desktop with a spindle in July of this year and spend a significant amount of time cutting a spoilboard that has dowel holes, threaded inserts, wedges and fences thanks to the help Scott Plaisted and others on this forum.

I am now trying to cut one of the sample projects from the Vectric forum. It is the Mother's Keep Sakes project that is a VCarved box. I'm making it out of hard maple for my Mother's 80th birthday.

I cut the lid and the VCarving went well, however the profile cut using an Onsrud 57-910 down spiral end mil, that I got with the ShopBot starter set, left a very scalloped cut on the edges.

I decide to create some test cuts with that cutter to find the best speeds and feeds. According to Onsrud the chip load for that bit and hard wood should be .005 to 007. I created some test cuts in that range in hard maple and hoped that I would find a speed and feed that were acceptable. Unfortunately after making twelve test cuts I can't say that any of them are very good. I'm pretty frustrated!

I'll attach the VCarve file that has my tests. They are labeled 1 Test 57-910 1.7 .5 10K, 2 Test 57-910 1.9 .5 11K, etc. The numbers represent feed rate in IPS, plunge rate in IPS, and speed in RPMs. I'm using a cut depth of 1/2 of the cutter diameter which is .125.

I would really appreciate any help that I can get.

Thanks,
Steve

[ssflyer]

Hi Steve,

I had to look up Eastvale, even though I've been through a lot of times!

Looks like you are off to a good start, if you mic'd the bit as it shows as a 0.248".

This can be a little frustrating when starting out. The chipload tables are a good suggestion. I don't have a desktop, so can't really chime in here on good speeds/feeds for you, but I run that bit all the time (Actually one of my go-to bits for profiling) and get really clean edges, even on some pretty weird curved/angled pieces.

I don't run much hard maple, but I just finished a bunch of walnut, with the same bit, 0.8" thick in 2 passes at 10,500 rpm and 6"/sec. and it came out very well.

Un-intuitive rule of thumb - run as slow RPM and a fast feed, until the edge quality suffers, then back off one of them until you are running as fast as your machine will cut, with an acceptable finish. When the cut's done, you should be able to grab the bit without getting burnt.

[Brady Watson]

Try 1.2, 0.7 IPS @ 13,000 RPM. There is NO WAY the tool can go the speeds you have set on those smaller parts (SB3 will ramp the speed down for you - but this is not ideal). Your car can do 100 mph, but probably not more than once in a parking lot...Cutting small parts at even 1 IPS can be considered way too fast depending on the part, material and hold down. Limit step down to no more than the diameter of the tool for hard maple.

Hard maple needs lower feeds and is very RPM sensitive. If burning, pull down the RPM. Keep an ear out for it sounding labored & make sure you have good hold down.

If you have ears to hear (an acquired skill of observation), the tool will tell you exactly where it wants to be in terms of speeds and RPM.

-B

[shilala]

It'd be really nice to have an example of what a good sound is when bits get into the wood at a good feed and speed.
When I started, I broke a few bits, mostly from pounding them into the material or forgetting to zero my z. Then once I ironed that out, I just watched and listened at Brady's suggestion. I leaned on the chipload chart for about five minutes just to see if what I thought was good fell inside what the factory said was good.
I just have a router, so if I get into a project and don't like the sound I can click it up a notch or down a notch while the project is running. I don't know that I've ever gotten past using the two lowest setting on the router.

[scottp55]

Steve, Didn't have a large enough scrap to really get into it, and my bit is getting a little long in the tooth so I've been using my Centurion, but you needed starter bit, soo..
I just made 2 rectangles and ran inside and outside cuts(so some of what you see is the waste side). My last setting was 2, .5,12.5K at .09"pass depth in the database, but I thought I had changed it for a specific project by mistake, so went to .1235(1/2 diameter). AND as Brady said she didn't like it.
I wanted to keep all cuts at 2IPS for comparison because it was only 3X6" scrap. Original setting cut great, but bit was a little too warm for my taste.
TRY 2, .5, 10.5K at .09" pass depth, climb cut, straight 1"ramp(inner rectangle surface). Your bit is newer than mine so RPM may vary(Just keep your hand on the VFD and adjust up or down without LOOKING at the speed,BUT looking and listening to the cut. Should have a tiny bit of squeal when she ramps down for sharp corners).
Results may vary
Good luck! (Oh! Maple is fairly figured so looks in places like chattermarks but it's not)

[Steve Wonser]

Thanks everyone for the suggestions. I really appreciate it.

I tried Scott's settings, which worked great for him. I used 2 IPS Feed, 0.5 IPS Plunge and 10.5K RPM. I set the pass depth to 0.09. The cut was outside using a climb cut with a 1" ramp. Unfortunately, I had the same results as before with the edges being scalloped, actually a pretty cool texture if that was what I was going for.

I tried Brady's suggestion of 1.2 IPS Feed, 0.7 IPS Plunge and 13K RPM. I left the pass depth at 0.09 and did the same cut as with Scott's settings. The bit screamed pretty loud, but I let it finish the cut and it came out good!

Next I tried Brady's setting only I played with the RPM a little. I slowly lowered it and noticed the bit screaming wasn't as bad as before. As I lowered it more I got kind of a low pitched grinding sound so I tweeked the RPM up a little. I think I ended up at between 12 & 12.5K. The cut was just as good as before only with slightly less noise.

The weird thing is the chipload for the settings Scott gave me (2 Feed and 10.5K) is 0.00571, which is in the range specified by Onsrud (0.005 to 0.007). The settings that worked for me (1.2 Feed and 12K) have a chipload of 0.003. It makes it hard to know what values to test with. I guess lots of experience with different materials is best.

Thanks again for your help!
Steve

[Burkhardt]

If you do not have good cuts at any of the suggested settings, maybe it is not the speed or feed which is the problem. Can it be that you have some play in your machine or spindle? In my experience hard maple is not that special compared to other hardwoods.

I do not pay much attention anymore to chip loads. I run small bits (up to 1/8") at 12k to 18krpm, medium size ( 1/4 or 3/8") at 10k to 14krpm and larger bits slower if I can (but the 3hp spindle gets quite weak at low rpms just when needed for large bits). Then I fine tune the speed by ear. I abandoned program controlled vfd speed and adjust with a hand knob.

With these speeds I can run anywhere between 1 ips and 6 ips (the max I trust my machine) and get very clean cuts. Much lower than 1 ipm risks burning the bit/wood. For large cutouts I go rather fast and for very detailed cuts I go on the slow side of the mentioned range since the machine won't come up to maximum feed rate anyway. The small bits are also limited to 1.5 or 2 ips at 1 diameter depth or they may break in hard wood. 1/4" and bigger can go much faster.

[scottp55]

Steve, Glad to see you're getting comfortable enough to play with it and I agree with G. that I only look at chipload calculator as a suggestion for totally different bits than I've never used before.
I only changed to a climb cut yesterday when I notice my wasteside cut was cleaner than the workpiece side. About 90% of my cuts with Downs is conventional. Also noticed my house carpenters writing on that scrap which places it at about "96. Thing I'd try next is can you get back up to 1/2 diameter or greater pass depth. No idea why my setting was at .09" except I was cutting quilted last week and maybe hit apply, but my CenturionFEMLH is at same pass depth but 1.1,.5,10K which is Teak/Jatoba speed.
Thing is , whatever works--Works. Keep an eye on your chips and feel the bit after a short time(should always be able to keep your finger on it) for temp. Listen like you did and the bit will usually tell you, a hand on the machine will tell you about small vibrations that can affect cut. Also found that some move speeds are smoother than others even under No load, set your radio buttons for a couple long X,Y moves and run through the move speeds and find the smoothest and roughest setting and write them down and try to use the smooth ones(hand on machine frame for vibration/resonance).
GOT to try Bradys settings now
Nothing is written in stone, and it can change from board to board, be glad you have a spindle and can reach around and tweak it.
My Downs are the only bits I ever have to use ear protection on

[Brady Watson]

Every material is different - Even "maple" as there can be some that machines better than others depending on the grain etc.

Not that long ago, there was nobody around to poll what the baseline speeds were for cutting xyz material. You just had to figure it out on your own.

Steve - ya done good. The key is to get in the range & then tweak the move speed or RPM as needed until you can see & hear that she's in the sweet spot. If you are cutting large rectangular parts, your speeds may be different (and even your VR settings) compared to cutting something very curvy and convoluted. Set your baseline speed - I do like MS,2,1 & 13,000 as a baseline...then feather the RPM up or down while it is cutting until I am happy with the overall results.

When a tool 'screams' it is usually because it is not taking a big enough bite to keep the tool from 'slapping around' at the tip. This is usually cured by lowering RPM or increasing the MS. I rarely run at chipload unless cutting plastic or metal. Tool life doesn't matter to me - quality does. It makes no sense running chipload if you can't hold the part down. By lightening up chipload you keep the parts from moving at the expense of some tool life. Sometimes it is a make it or break it proposition...

-B

[Ger21]

........... The cut was outside using a climb cut ..................

The scallops are a result of climb cutting. With wood, conventional cutting will almost always give a better cut than climb cutting, provided that there is wood on both sides of the bit. If there is no wood on the outside of the cut, then tearout can become an issue.