Feed speed

[w_kerry]

Question: How fast can a PRT standard with basic software run without sacrificing accuracy(assuming that the depth of cut,bit diameter, and type of material being cut does not slow down the 3hp spindle).

[Brady Watson]

It is unlikely that you will bog down a spindle before you stall a Standard machine. Depending on what you are cutting, max speed on a Standard is between 4 to 6 IPS, but there are all kinds of things that come into play. Depending on what you are cutting, you may be able to cut even faster than that. My street bike will do 95 MPH in 2nd gear...but there isn't enough road on my street to go that fast & stop, if you catch my drift.

-B

[w_kerry]

Brady,
Since I posted this question,I have spoken to Shopbot who warn me that I may lose steps in my program if I go above 2in/sec.Are they being overly cautious or can I expect to be able to go faster. I will be cutting 3/4 plywood radiused cabinet parts that must be right on the money for everything to fit together.

[w_kerry]

Ran my first program today, cutting 3/4 plywood plates on radius. Cut full depth in single pass using a 3/8 dia. single flute carbide bit.A 3.5" plate ended up measuring 3.625.Granted the bit had some milage on it but the bot cut right through with seemingly no problem. Will it be necessary to step cut with a brand new bit to solve this deflection error? By the way, my speed was 2.0 in/sec @16000 rpm

[evan]

1. Measure the actual dia. of your bit and enter that into your tool profile before creating the tool path.

2. 3.5" dia. plate is fairly small how are you holding down? Is the material moving?

3. There could be some deflection of the bit. Cut an identical plate but in the opposite direction (a climb cut if original was a conventional cut or visa- versa) and check to see if the measurement is off in the opposite direction. If so, then do a rough cut in conventional leaving a skin (.75 material only cut .73 depth) on the bottom then do a final cleaning cut (actual size and depth) with a climb cut.

[w_kerry]

EVAN,
The part is actually a 3.5"x90" radiused plate for a stud wall in a reception desk. I ran the program air cutting and barely skimming the table. The cut was 3.5" on the money. When I made the cut full depth on the plywood,the bit deflected .0625 at the beginning of each cut.Is this normal or perhaps is my machine worn out? I bought it second hand and it's about 10 years old. I was told it didn't have that much use on it.

[Brady Watson]

Kerry,
Why do you need to cut in a single pass? Not a good idea on a Standard.

-B

[w_kerry]

Brady,
Ive become used to a "big iron" machine at my daytime job, so I guess I will need to readjust my methods to suit the situation.I will next try a two step cut with a 1/4" down cut spiral bit. Since I'm taking so little material out with this bit,can I cut at a faster speed,say 4-5 in/sec?

[Brady Watson]

You have a couple things to consider. 1st & foremost is losing steps. As long as you are not losing steps, you should be OK in 2 passes. It's a shame you didn't get an Alpha. It would give the big iron a run for it's money. The 2nd thing is cutter deflection. If you went up to a 3/8" bit you would only add .125 to the kerf, but increase stiffness by 40%. Bit deflection can be a major source of off-spec parts.

While it's great to cut fast, my focus has always been on quality & accuracy. Many times this means slowing things way down. It is hard to say what speeds you can reliably cut at, since many factors come into play. Plywood cuts differently than hardwood or MDF, bit geometries and even manufacturers yield different results...even your hold-down method will influence how the part is cut. Adjusting the VR of the tool can make all the difference in the world.

Do lots of testing and observing of your cuts. Make a chart or log of your findings.

-B

[w_kerry]

Brady,
My line of thinking concerning bit selection was that the error of my parts was due mainly to the shopbots mechanical tolerances and not the bit deflection. After all,I am able to cut full 3/4 depth with a 1/4 spiral bit on "big iron" with no perceivable deflection. If bit deflection was the problem, I should see it in that application as well.Consequently my choice of a 1/4 diameter bit is an attempt to reduce the lateral cutting forces that are giving me the error.
Right now I have a software problem that must be addressed before I can do any more testing(hopefully I'll be back up today)
One other concern - I don,t mind so much slowing things down if it results in accurate parts,but I have experienced in certain instances premature bit dulling due to insufficient feed speed.Do you have experience with that? Can premature dulling be reduced by lowering the bit rpm? Also what are you refering to when you mention "vr"?
Thanks much for all the input.

[beacon14]

Kerry,

1/16" of sloppiness is not unheard of on an older machine when pushed near to its limits like that. (If it's 10 years old it's probably a PR, not a PRT) You can probably minimize the amount by tuning the machine but you wont likely eliminate it entirely if you want to cut in one pass. The way I cope with this is detailed in my column (http://65.36.212.143/notes_from_the_sandbox.htm#Almost%20There) on the ShopBot web site.

For plywood I usually make the roughing cut in two equal depth passes, then the final cut at full depth. That way you can utilize the fastest speeds your machine can handle, but that may still not be fast enough to prevent premature bit wear with an older, standard machine.

[Brady Watson]

Kerry,
I missed the PRT part...and thought it was a PRS Standard machine. So, yes SB was correct in telling you that it will cut a max of 2 IPS @ full depth. I never tried cutting full depth on my (days gone by) standard PRT. It sounds to me like a 4G upgrade would be right up your alley & would cut up to 6-8 IPS & Jog 8-12 IPS...Something your PRT will not do at the moment.

RPM & Move speeds boil down to chipload. Give the chipload calc under the Tools menu in SB3 a whirl to get dialed in. This will help you to prevent pre-mature dulling of your tools.

VR = Values Ramping - which can help tune your tool for the type of work that you are doing.

-B

[conceptmachine]

If you are using a solid carbide bit and getting 1/16" deflection it is NOT the bit it is the gantry.I cut steel all day at my shop on my vmc and the worst deflection i have ever got without breaking was.007 per side,this is what seperates the heavy iron machines from shopbot style machines you dont have to over compensate for gantry deflection when setting up tool diameters.

[gpari]

I agree with Shawn. It is not the bit flexing, it is the gantry. I also doubt that it is mechanical "slop" or tolerance problems. Unless of course the gears are worn or somethings loose, in which case, it's not the machines fault. The gantry on my machine will flex upwards of .050" with just light pressure from your hand. Put a lever arm on the end of the router (ie. router bit) and you can flex it pretty good with not much force. I suspect the newer PRS upright style gantry is a bit stiffer.