Rugged enough to cut thru 1+" hardwoods?

[Forum Admin]

SOS! Just how rugged are the bots?
Would like someone to talk with who uses one for a smaller type production shop. We build curve stairs. We are CAD users. We currently send dwg files to a local CNC Millshop for making templates. We use hand routers to follow these.
Wouldn't mind spending 20K or so for value and ruggedness. Posted by Kevin. Moved here by Forum admin

[richards]

Shopbots are rugged enough to cut aluminum, so they can easily cut hardwood. However, like aluminum, you'll probably want to take several shallow passes instead of trying to cut all the way through in one pass. There are a lot of factors that determine the depth of cut, such as the router/spindle that you use; the diameter and type of cutter that you use; the feed speed and the spindle/router speed; the hold-down method; and of course, the type of wood that you're cutting.

[harryball]

I accidentally cut a piece of 4/4 red oak in a single pass. I was using a 1/4" up spiral solid carbide bit. I say accidentally because I intended to cut in 4 passes. I originally cut the test template in 3/4" MDF in a single pass. When I had it tuned I re-did the toolpath and set the cutting speed to 1 ips but neglected to reset the pass depth. After a brief panic I watched as the Alpha with a 4HP HSD spindle cut the part. The edges had to be cleaned at the spindle sander but otherwise it turned out fine. The part was screwed to the table and if memory serves my RPMs were around 11000, which was high per the chip load calculators math.

I'm a newer bot user but my experience is mounting. Such "green" actions as above did no harm to the bot which didn't appear to strain or be harmed in anyway.

I don't know what others are running but I've been taking 3 passes at 3 ips at 12,000 RPM on clean (no large knots) 4/4 red oak. I'm probably being conservative.

Robert

[patricktoomey]

I cut 1.5 inch thick oak and hard maple into radius edging for counter tops. I usually cut them with a 1/4 inch. up spiral at 3 inches per second, 1/4 inch stepdown, 10,000 RPM using a 5hp spindle. The ShopBot is rugged enough to do this all day with no problems at all. I have cut wood like this with a 1/2 inch stepdown and a higher RPM like 12,000 but the edges are sometimes a little rough that way and it's putting more stress on the bit. Using a 3/8 inch bit should allow for faster/deeper cutting as well.

[rhfurniture]

57mm (2.25in) Utile chair rails no problem.
But I bandsaw them to rough (+3 to 4mm) then cut them 2 pass with a 1 flute 14mm X 50mm RT cutter max rev at 20mm second feed. I have a prt + 2hp Bosch router.

[bcammack]

We're cutting faucet holes and basin cutouts for bathroom vanities out of a 3cm acrylic-modified polyester material that is 65% alumina trihydrate powder. The stuff is hard and dense.

We're running the 5hp Colombo spindle with a 1/2" Onsrud solid carbide, heavy-duty two-flute chipbreaker upspiral bit. We can run at nearly 1 inch-second through it in one pass at about 6750 RPM. Any faster and we burn up the tool's edge. (we are on the cusp between routing and milling with this material) Amp draw is between 8 for an new bit and 12 for a used one.

A bit is good for about a hundred or so sinks before it's toast and we toss it. Finish isn't great, but we consider this a "cutting" or "sawing" operation, so there are processes downstream from the Shopbot to sand or finish route out the "saw marks" from this process.

Here are some pix.


8678

The pneumatic rams are on the "back" of the table. The backstop/fence is on the "front" of the table. A laser projects the sink centerline across the table so the operator can slide the blank vanity top onto the table, line the mark on the blank with the laser, flip a lever to lock it down, and push the "run" button on the touchscreen after selecting the correct sink and faucet combination. The production line is configured to run 100-120 tops per shift.


8679

The lever to the left of the touchscreen controls the compressed air rams the clamp the vanity top against the backboard.

[Brady Watson]

Brett,
Looks like a nice setup.

Your 5HP Colombo is not designed to run production at 6750 RPM. You are running the risk of burning out the brushes prematurely and other parts as well. It is designed to run between 12,000 and 18,000 RPM. If you lighten up the stepdown, you can move the CNC faster while maintaining a good edge and increase tool life.

In terms of tool life, I would encourage you to look into PCD diamond coated tooling for this application. They cost more, but in applications such as these, tool life is 10 to 15X that of standard carbide end mills and bits. I use diamond bits exclusively when cutting carbon fiber, kevlar and FRP materials where material hardness (ability to resist scratching/cutting) is an issue.

-Brady

[richards]

Brady,
I think that we're comparing apples to oranges here. The Colombo, unless I'm totally mistaken, is a 3-phase motor without brushes. It is true that torque - on most models - is constant between 12,000 and 18,000 RPM, however, it is designed to run at any speed, as long as the linear reduction in torque at speeds less than 12,000 RPM is acceptable. The cooling fan is independant of the spindle speed, so there is no reduction in fan RPM when the spindle is run at slower speed. I almost never run my spindle slower than 12,000, so I don't have first-hand knowledge about extra heating when the spindle is run at high current levels at slow speed; however, I have drilled a 'zillion' (defined as somewhat more than 1,000) holes at 3,000 RPM without any problems.

I totally agree with you that running multiple passes at shallower depths per pass would be the way that I'd run the job - but - I've never cut that kind of material, so maybe, all things considered, Brett has found the best compromise, given his shop and tooling conditions.

Brett,
That is a first-class setup. I wish I had room for something like that in my little shop.

[mikejohn]

Brett
Interesting to see a Shopbot set up for a single operation. How long have you been running this operation? Have there been any problems (or benefits) continually cutting in just one area?
I like the position of the cut screen. It seems it stays right out of the operators way.
Do you feed and remove stock always from the right?

..............Mike

[pete]

Brett,

Great setup. Any chance of seeing pictures of the rams and the backstop arrangement? Thanks. Pete

[harold_weber]

Brady, if there are brushes in the Colombo 5Hp spindle, can you tell us the instructions for the process used to inspect/change them??

[nappy1]

Brett,
Your Shop is too clean..........

[richards]

Sorry, but I got mixed up on constant power vs constant torque. This quote is from the PDS Colombo web site:

"Power Curve

Colombo Electric Spindles are available in either Constant Power or Constant Torque. Both types offer advantages depending upon the operating speed for the cutter(s) used in your application.

Constant Torque electric spindles suit applications where maximum cutting power is required near maximum spindle speed. Their torque is constant so power increases steadily from zero at zero speed to full power at full speed.

Constant Power electric spindles provide flexibility for a wider variety of cutting tasks. They deliver more power at mid-range speeds but less power at maximum speed than constant torque spindles. Typical constant power ranges are 9000 - 18000 rpm, 12000 - 18000 rpm or 18000 - 24000 rpm. The selection depends upon the operating speed for the cutter range & material type."

[Brady Watson]

Harold,
I've got the instructions all typed up over here...you guys are too much!

While I never profess to be an expert on AC or DC motors, I DO know that the 5HP Colombo has very little torque at 6750 RPM. I also know that PDS recommends cutting wood, plastic & composite materials at 12,000 to 24000 RPM on these models. They also made it very clear at the Jamboree that the Colombos that SB sells are not rated for drilling, when I spoke to the rep. Both of these points should be made clear if warranty service ever became an issue. I can drive my V8 Mustang in 4th gear @ 25 MPH, but it isn't too happy when I start climbing a hill or mat the pedal...

In spite of 'official recommendations', I drill at lower speeds and sometimes mill at lower speeds. I would never recommend to a customer that they run their spindle in production of ANY material below 10,000 RPM. That's just me...and how I would run my tool. If you paid for it & feel OK with your settings, by all means go for it!

-B

[richards]

Brady,
That's the beauty of a Shopbot. It can be used in many 'non-approved' ways. Brett uses his to do something that works for him, even though his technique is 'non-approved'. I drill a zillion holes with a spindle - but they're only 1/16-inch deep using a 1/8-inch bit. In other words, they're spotting holes, which are used to make it really simple to drill the real holes manually with an air drill after the part has been removed from the Shopbot. I'd like to be able to drill the actual holes on the Shopbot, but, as you mentioned, the bearings in the Colombo spindles don't like heavy axial loads, so I found a way to get the job done as efficiently as the tools allow.

One other little note. You listed PDS's recommendations of speeds from 12,000 to 24,000 RPM. Unless I'm mistaken, speeds higher than 18,000 RPM require ceramic bearings - which are not normally furnished in the 3hp and 5hp models. I've been told that running the spindle at speeds greater than 18.000 will burn up the bearings in a very short time. To keep that from happening on my machine, I've programmed the VFD to limit the top speed to 18,000 RPM. Is it advisable to run the 3hp and 5hp spindles at 24,000 RPM?

[Brady Watson]

I'm pretty sure all the ones SB sells these days have the ceramic bearings (not 100% sure so don't quote me)...I'm pretty sure my 5HP has them...I remember reading the handwritten literature for my specific unit when I first got it.

By the way...since you just want to spot the locations, a spring loaded center punch with a mount adapted to the Z works really well....Just don't chuck it in the router


-B

[richards]

Brady,
Thanks for the suggestion about a spring loaded center punch. The next time I'm in the mood to 'fix-up' my Alpha, I'll look into that type of device.

I looked over the documentation on my spindle and couldn't find anything about the bearings. However, I found something else in the documentation from Colombo that makes we scratch my head: "Please, use fast feeds approaching the tool to the piece, but limit the machine feet (sic) to 2 mt/min during the impact between the mill and the piece to work." Admittedly, their translator should have had someone proof-read the document. I think that they mean that the feed speed should be limited to 2 meters/min when entering the cut. That's about 1.3-ips.

I knew about the limitation of greatly reducing the Z-axis feed speed (unless ramping into the cut), but this is the first time that I read about a limitation on the feed speed when entering a cut from a radial direction (X and Y axes). It makes sense when you consider the "shock" created if you were to "slam" the cutter into the work piece.

I've sent an email to PDS Colombo asking for specifics on the bearings in my unit. In most respects, it doesn't matter because I rarely run the spindle faster than 15,000 RPM. Depending on what I'm cutting and the chipload that I want, feed speeds in the 5-8 ips range only require moderate spindle speeds. For example, to cut MDF with a chip load of 0.015 at 7-ips feed speed and a 2-flute cutter, calls for a spindle speed of 14,000 RPM. If the piece has lots of tight curves where the Shopbot is spending most of its time ramping up and down, the actual feed speed might be closer to 2-ips, which would mean a spindle speed of only 4,000 RPM. (That's why I always keep some 1-flute cutters on hand.)

Of course, some of this is only academic. If you have work to do and you're charging enough to maintain the machine, running full-out would probably be a lot more profitable than nursing the machine to save the bearings. Spindles are costly, but they're only a small part of the overhead in a typical shop.

[bcammack]

Brady,

Do you have a link for those diamond coated tools?

This material tends to put a lot of heat on the cutting edge. We've struck this compromise through experience with the Onsrud 60-950 after considerable experimentation. We actually start in the upper 7K range with a fresh bit until the edge is knocked off the tool otherwise the motor can't produce enough torque and we get bad chatter. This material is a bit more abrasive than we think it should be. Suspicion is that the supplier is using some less expensive calcium carbide to dilute the alumina trihydrate and shave some costs.

We played with doing a couple of passes, stepping down into the material, but found that the net effect was to wear out a smaller portion of the tool faster in proportion to the depth of the plunge. Tooling cost made it more practical to wear out the whole 1.25" edge of the tool by doing a single pass cut. (tool change time is a cost factor, too, when you're trying to do 100 tops per shift)

Now we just slog along at 0.8"/second at full depth and are satisfied with getting a 100 tops out of a $70 bit. That's a bearable cost.

I suspect we are really at the hairy edge of the ShopBot's rated capacity.

Thanks for the complements on the setup, guys. I'll try to post up some pix of the work surface itself.

I guess the point of my original post was, if it can cut this stuff, it should have nooo problems cutting hardwoods 1" thick.

[Brady Watson]

These are expensive, but they are the best: http://www.robbjack.com/html/pcd.html

I use these:
http://www.osgtool.com/catalogmill.asp?MillType=Square&ProdListNum=7040&P rodNumPos=1

The performance is really incredible and the cut quality is better than a standard coated tool since the diamond coating actually polishes the edge. There are a number of other manufacturers out there that sell PCD coated tools. Be aware that many sell DLC (diamond like coating) that are the cubic zirconia version of PCD...and they only offer a marginal increase in performance and duty compared to standard carbide.

-B