Speed and Feed again

Discussion about the CNC Shark Pro Plus HD

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
GrandpaB
Posts: 45
Joined: Sun Apr 22, 2012 7:45 pm

Speed and Feed again

Post by GrandpaB »

Yesterday I posted the following on the Vectric forum.

"I've not been happy with the results that I've been getting cutting parts from 1.4" pine. I've been using a 1/4" up cutting end mill running at 17,000 rpm and 100 in/min (typo in the original said in/sec). A concern is that the bit was designed to cut only 1.25" deep. Looking for a new bit I stumbled across RobbJack. On their web site they have a speed and feed calculator. When I entered the parameters for my Shark HD CNC router it suggested that I run at 25,000 rpm and 200 in/min. Has anyone run at those conditions and has any one had experience with the RobbJack calculator? From what I've seen on this forum those conditions seem a bit extreme."

I received two replies. Bob said that he gets good results at 13,000 rpm with a Porter Cable 7581 and 200 in/min on most of his wood projects. Russell said that his Shark Pro Plus had a hard time cutting 1/8" depth with 1/4" endmills. It would tend to chatter and wander. He felt that there was too much flex in the Shark gantry, etc. He uses a 1/2" compression bit and cut 3/4" depth at 400 ipm.

I don't know what CNC systems they are using, but is anyone sucessfully runnning the Shark HD with a 1/4" end mill above 100 in/min?.

ccarv
Posts: 6
Joined: Fri Feb 15, 2013 10:54 am

Re: Speed and Feed again

Post by ccarv »

I'm running 200 ipm speeds and .150 deep bites with a .250 ball nose mill at 18,000 rpm, but I'm cutting bone dry red cedar, which is almost like cutting balsa wood. According to the Janka scale, your pine is softer than cedar.

4DThinker
Posts: 951
Joined: Wed Jun 27, 2012 9:00 am

Re: Speed and Feed again

Post by 4DThinker »

The one variable you haven't mentioned is Pass Depth. Ideally, it is the combination of bit diameter, pass depth, and feed speed that have to be balanced against the wood/whatever being cut. You want the bit to have a chance to remove the cut off chips efficiently enough to not get hot during a cut. The heat generated gets removed with the chips.

Finding the perfect feed speed to run any bit is very much like magic. Change the wood being cut and you'll need to change the speed. Change from an upcut to a 2-flute straight bit and you'll have a whole new calculation to make.

I tell my students (we have a Shark HD 2.0 in our furniture design shop) to start any cut with the feed speed slider at 50%. VCarve generally has every bit defined to run at 100ipm with the pass at 50% of the bit diameter. If the bit sounds good and isn't vibrating or chattering as it goes then they can slide it up some. There IS a great deal of flex in the gantry assembly of the Sharks, and you simply can't run bits the same speed as you would run them on a large Multicam CNC.

Eagle55
Posts: 788
Joined: Sun Nov 20, 2011 8:44 pm

Re: Speed and Feed again

Post by Eagle55 »

I hear people cutting at 100 ipm all the time but to be honest and contrary to the pack, I wouldn't even consider this. Personally, I am after a good cut that leaves little additional work before going to finish as opposed to saving seconds or even minutes in the carve process and having hours to clean it up and get it acceptable to finish. Yes, the gantry has flex and if you push your bits too hard you WILL see this in distorted carves, bad cutting, chatter etc. In other words, bad things will begin to happen. If someone is using 100 ipm and having good success, I say more power to them, but I have not see this to be the case in what work I have done so far. I typically design with a default speed of 100 ipm and then will actually run the cut at 30-50% on the FRO slider. Sometime I change a bit in the database to design with lower. To the indications that say 200 ipm, I can't imagine that working for them, but hey, if it is, it is. I'm not challenging them, I'm just saying not on my machine would you ever get away with it. (I have the HD) I use a PC 690 router with a fixed speed of about 25,000. I wish I could slow it down and have bought a PC 892 for this purpose, when the bearings are finally gone in the (2nd) PC690. For bearing life I am going to use slower rpm and see how that works. (while I learn how to change the bearings in my 2- PC690's) The old story goes that if it works well for you, stick with it, but some of the numbers I have heard seem unrealistic to me with my limited experience in CNC. My methods work best to cut slower, take shallower passes and not try to exploit the speed ability of CNC. I think you will have better luck taking advantage of the ability to do things you can't do any other way, than if you try to do jobs at lightning speed because it is a "computer". Yes, the Shark can do it lightening fast, but you will soon feel like the gantry is made out of spaghetti and you will likely be posting about how the round holes are egg shaped and distorted and straight lines aren't straight and it takes you 5 hours to sand a 3d carve that only took you one hour to carve etc. These are just my opinion.... and I'm sticking to it. LOL

Roger
CNC Shark HD ~ Control Panel 2.0 ~ Windows 7 & XP
Located in West Tennessee near the Tennessee River
http://www.eaglecarver4.com

TDA
Posts: 44
Joined: Wed Apr 13, 2011 10:33 am

Re: Speed and Feed again

Post by TDA »

Unfortunately there is not an easy answer for this. You have a couple of competing issues and multiple ways to deal with them.

First, you have what the tool wants to cut at. This is a combination of the material you are cutting and the tool geometry. Basically you have to keep the tool engaged in the material while not exceeding it's ability to remove material. This is a complex issue. If you cut too slow you will end up with odd little chatter marks or burrs on the top of the cut. Way too slow and you will end up burning your tool/material and decreasing the life of the tool. Go too fast and you will have a burr and chipped up surface on the wood. Go way too fast and you will end up with a broken tool. Keep in mind that this can change greatly depending on the material being cut.

After you get that down then you have to deal with what your machine can handle. This is usually an issue of deflection. This is an effect of the force of the cut on the tool and the machine. Basically the deeper you cut or the more material per rev you take the higher the forces on you machine and tool. Again this can change greatly with a change of material.

So as you increase your feed or decrease your RPM you raise your material removed per revolution. Which helps the tool cut well but increases the forces exerted on the machine. The usual way to deal with this is to increase your feedrate, lower your RPM, and take a shallower pass. This allows you to cut with a decent engagement while keeping the deflection down.

There are other issues as well. Material sheer, tool impact, engagement time, variable geometry, router torque, backlash, machine acceleration, ect. All these also have an effect but they are much more subtle then the two listed above in most situations.

Here are a few good rules of thumb. The more flutes, the higher the feed. The bigger the tool, the lower the RPM. If your tool is squealing, your RPM is too high. If your cut material looks like powder, you are going too slow or your RPM is too high. If you machine is cutting extremely quite, your tool is broken.

I don't have nearly the time I used to so it's hard to get on. But if I can be of help let me know.
John Torrez
Think & Tinker / PreciseBits

Post Reply