Feed and speed for Onsrud 60-113 Compression Bit in Baltic Birch

[johnsontoddr]

I'm about to cut half inch (0.472 inch) baltic birch on a Desktop Max using an 1/4" Onsrud 60-113 two flute compression bit. According to Onsrud the chipload should be .015-.017 for soft plywood and .014 to .016 for hard plywood. Since the Desktop Max maximum feedrate is 240 in/min, I have to set spindle speed at 8000 rpm (I have the industrial spindle). This seems quite slow and is considerably slower than I've seen others mention in the forum.

I'm not sure whether baltic birch is consider hard or soft plywood, but the difference it makes here seems negligible. If I use the .014 chipload I can raise spindle speed to 8500 RPM.

So I'm looking for feedback from anyone else using this (or a similar) bit on a Desktop.

Todd

[scottp55]

What pass depth does bit require to get below the upcut portion?

[Gary Campbell]

Todd....
Some starting points:
If the upcut section will allow a 2 pass strategy (.25 per pass) then I would go with .005 chipload. Feedrate of 2 ips and 12K rpm.
IF you have to go deeper to keep the downcut section engaged, the go with one pass or an onionskin at .004 chipload. 2ips and 15K rpm.

If your geometry has numerous short sections and you find you must reduce feedrate, adjust rpm down proportionally.

Most published chipload numbers are NOT for desktop sized machines.

[johnsontoddr]

The Onsrud 60-113 is a mortise compression bit with an upcut flute length of .188 inch. I'm using it to countour (I think vcarve calls this a profile cut) two fairly large shelves for a monitor stand after pockets are cut with a downcut bit. I have set up the toolpath (using fusion 360) to use two passes where the bit plunges to .25 inch before moving to the profile. Second pass also plunges away from the part before cutting the profile. I force this to go a little below the part depth to ensure that the upcut portion of the bit fully engages the bottom of the part. The geometry is mostly straight but there are a few tabs to mate to other parts. Those have dogbones added. I also added small tabs to hold the parts in place, but I put these only on the non-show edges.

I've considered using a finishing path with the first two passes using climb cuts but leaving a skin around the parts, then making a final full depth conventional cut. However, I'm not sure how this would work with the dogbones, which are the exact diameter of the bit.

The Onsrud chipload table does seem really odd for this bit. Most of the chiploads for their other 1/4 inch bits are in the .00x range and work out to 180 in/sec at 12000 RPM. This is one of the few that is at .0x. The other bits I've got are all part of the shopbot starter kit, so I've been able to use Vcarve's shopbot library to look up the feeds and speeds. The 60-113 is not part of that.

I'm going to give your numbers a try today and then see how the cut looks and how warm the bit is after the cut.


29425

[johnsontoddr]

I just reviewed this ShopBot video on cutting plywood by TJ Christiansen (https://www.youtube.com/watch?v=XteEyLYvtXA). He also recommends 2 in/sec and 12000 rpm for the 60-113.

[dlcw]

I use two-flute compression bits all the time on 5/8" Appleply (baltic birch but in 4x8 panels made in the USA). I cut at 5IPS at 13K rpm. 5/16" each pass. I get good clean cuts and the bit doesn't scream (indicates a hungry bit). I cut about 200 sheets of the stuff per year and this configuration has worked well for my machine. Just remember on a compression bit, you will need to plunge at least .25" before you start ramping. Otherwise the upcut on the bottom of the bit will splinter the plywood veneer.

johnsontoddr - what you say about the climb then conventional cut is right on the money. There is enough inherent slop in the machine (not a lot by woodworking standards) but enough, that the climb cuts will push the bit away from your cut line. Leaving a 1/32" skin. Final full-depth conventional cut will pull the bit right to the cut line. Make sure you are only cutting 1/32" on the final pass. Don't use the process of cutting 1/4" per pass on the final cut. Cut full depth. I use the same climb/conventional cut method on plywood and solid wood. Makes for a cleaner, more precise final cut.

[Ajcoholic]

I'm about to cut half inch (0.472 inch) baltic birch on a Desktop Max using an 1/4" Onsrud 60-113 two flute compression bit. According to Onsrud the chipload should be .015-.017 for soft plywood and .014 to .016 for hard plywood. Since the Desktop Max maximum feedrate is 240 in/min, I have to set spindle speed at 8000 rpm (I have the industrial spindle). This seems quite slow and is considerably slower than I've seen others mention in the forum.

I'm not sure whether baltic birch is consider hard or soft plywood, but the difference it makes here seems negligible. If I use the .014 chipload I can raise spindle speed to 8500 RPM.

So I'm looking for feedback from anyone else using this (or a similar) bit on a Desktop.

Todd

FWIW I've cut more 12mm Baltic birch than anything else on my Shopbot in the past 5 years. I cut up several dozen sheets every few months, since 2012.

Early on I settled on a general feed speed of 240 to 360 ipm, rpm between 11500 and 12500.

Basically it depends what I'm cutting. But I run the spindle until it "squeals" going around corners, then reduce the rpm by 500

For larger pieces I set feed at 360, for smaller parts 240.

I usually do two passes - first climbing at a depth of .42 and second pass conventionally cut full depth plus 5 or 10 thousandths.

This has worked very well for me with a two flute 1/4" onsrud spiral or compression spiral. I find on an MDF spoil board a down cut spiral works as well for clean cuts and parts that are small less likely to move on the vacuum table.

[Gary Campbell]

Todd, et al...
This is a good lesson for those that are new at setting feeds and speeds. Any and all of the above numbers are accurate.... based on the limiting factors.

That with a big iron machine, mega horsepower spindle and major hold down, .015 is the optimum chipload for that bit.
Don has a full size alpha machine with a vacuum system and he cuts well at .012. He is a commercial user with years of experience.
Smaller machines will use .003 to .005, at least as a start point.

Remember that 1 ips @ 6Krpm, 2ips @ 12Krpm and 4ips @ 24Krpm are all .005 chipload.

Most of the tool mfgr's chipload charts will provide MAX chipload for a given bit. This will provide fastest cutting and longest bit life assuming there are no other limiting factors.

Just so you are aware, those limiting factors are hold down (yes, it makes a big difference) horsepower of the cutting head, rigidity of the frame and motion components and the power of the drive components. (motors, gearing and drives). Each of these, or in reality, each users combination of these will determine the chipload that works best for a given job on a given machine. The above combination PLUS variations in material densities AND bits from different suppliers gives unlimited "perfect" feed, speed and stepdown options.

That's why most will offer up a staring point, usually conservative, to allow the individual operator to tweak to his/her actual setups.

[johnsontoddr]

Great discussion. Thanks for all the feedback. I had been getting clean cuts on both sides of BB with a downcut bit, but lately I've been getting a lot of tearout on the bottom face. Either the bit is a bit dull or the spoilboard is not clean enough, or perhaps its just variation in the BB. Thus I decided to try the compression bit.

One more issue: I understand that I should not simply plunge the bit down, but if I ramp the cut, some of the profile will get cut with the upcut portion. How do you handle this? In fusion 360 it looks like I can predrill entry positions using a helical operation and then tell the contour toolpath to enter there. I've tried playing with lead-ins and the various parameters around that, but those don't seem to do much.

[johnsontoddr]

Don: will the climb cut at the stock perimeter automatically leave 1/32" due to the physics, or should I create the toolpath to leave a 1/32" skin then finish that with a second conventional cut at the exact stock perimeter?

[Gary Campbell]

Todd...
Due to the upcut section on the compression bit you will need to plunge straight in. They are designed to do exactly that, speed appropriate of course.

In most cases you can just set the directional change as climb first pass(s) and conventional last. No need to offset vectors.

[dlcw]

Don: will the climb cut at the stock perimeter automatically leave 1/32" due to the physics, or should I create the toolpath to leave a 1/32" skin then finish that with a second conventional cut at the exact stock perimeter?

You will need to create 2 toolpaths. First one is the climb cut leaving the 1/32" skin. Second toolpath is the one that cuts all the way thru.

Gary brought up a good point. Each machine will be slightly different. You need to spend the time dialing in what's best for YOUR machine. Other people don't have the same thing you do. So, take the time and experiment. Like Gary said I've been using my full size Alpha with vacuum gold down cutting commercially since 2009. I've spent time tuning it (read breaking bits) and figuring out what the sweet spots are for my machine. I cut well over fifteen hundred sheets of plywood a year on my machine. That doesn't include all the 3D carving I do for myself and customers plus all the hardwood cutting I do when making furniture. Each owner will have to do the same.

[dlcw]

Todd...
Due to the upcut section on the compression bit you will need to plunge straight in. They are designed to do exactly that, speed appropriate of course.

In most cases you can just set the directional change as climb first pass(s) and conventional last. No need to offset vectors.


Like Gary says here, you don't need to factor in any kind of offset in your cut. The final conventional cut will end up cutting about .001" - .005". At least that's what is is on my machine. Melmine is closer to the .005"