A few questions

[bandphillips]

Hello
I have recently acquired a shopbot and got it going. I am cutting 13/16 diameter holes, 3" deep. Alot of them. I am using a 1/2" x 4 1/2" straight cutter in circle pattern and stepping it down 1/4" at a time. I am only able to run the feedrate at 15 ipm. If I go any faster the bit chatters and ruins the hole. I'm pretty sure it is because it is because the bit is so long and is cutting so far from the collet. I am going to try a spiral upcut and hope that allows me to increase the speed. Any ideas on that?
Also does anyone have any idea if it is possible to increase the collet size to 5/8 or 3/4 so I can use a larger shank?
Last question. My machine has the capability to run 2 routers. I am thinking I can run both of them at the same time and drill 2 holes at once. Is it possible to run both of the z motors with the same input simultaneously?
Thanks

[bleeth]

Are you sure you aren't set to 15ips? That would be too high.
Also we would need to know what kind of Shopbot you have and what kind of spindles/routers are on it to answer.
What are you cutting? Straight cutters aren't usually used for wood products. An all upcutter may tear out at the top. A mortise compression bit could be better.

[adrianm]

What are you using to toolpath the job? Partworks or similiar? Just straight SBP code?

How are the toolpaths set up? Profile/Pocket? Ramps?

[bandphillips]

Hi Dave. It is 15 IPM. I am running a 48 x 96 Shopbot. Not the Alpha. I can't remember the model. Its made around 1999 or 2000. It has a Porter Cable 3 1/4 horse router with a 1/2" collet. I am cutting beech wood. I was thinking that the upcut would clear the chips out better and that the spiral cutting surface would be in contact with the wood at all times instead of the straight cutter coming around and hitting the wood every time. I am thinking that is making it chatter more.
Hello Adrian. I am using Artcam 2012. I am using the profile cut option. 1/4" stepdown. It actually steps down 5/16 each time I think because the previous owners changed the gears on the motors. I had to use trial and error for the finish depth to get to 3". Conventional cut. 30 IPM on the plunge. The router is running at the highest speed that it can at 26000rpm.

[bobmoore]

Bill;
If I were doing a job with a lot of holes I would have a 13/16 upcut bit custom made and just plunge the holes. You won't get a clean hole at speed even with the big iron machines if you are only enlarging it that small amount. Maybe you will have to peck depending on depth and material. You really should put more information in your posts if you want the best specific advise for problems. Bob

[bandphillips]

Thanks Bob. Any ideas on where to have a custom bit made?

[gene]

what type of motors does your machine have ? Maybe someone can give you the right numbers for that motor so 1/4 is equal to 1/4 and not 5/16

[bleeth]

So 1999 0r 2000 means a PRT. For drilling your router should not be running at top spin speed. Think about a drill press. As stated before a straight bit is not the right tool for this. You need to not only have a spiral for this, you also need to make sure you are using solid carbide cnc quality tools. You need to make sure your tool is not just continuing down the hole, but retracting between steps and evacuating the chips. If you don't get accurate depth steps without "guessing" then you have the wrong unit values for the motors and gear combo. The right one is easy to determine given your motor model and what pinion uyou have.
If you don't remember, write it down and post it later. The motors are likely 3.6/1 TH geared but to get the right unit value we need to verify the Teeth number on your pinions. If your holes are really sloppy with that kind of low speed then your machine likely needs adjustment as well, even with a straight bit. In general though, that low a movement with that high a spin will make dust and not chips and burn up your bit fast anyway.
Funny thing is, making a lot of holes like that is not really as easy as it may seem at first thought. A lot of factors have to be right to get decent results.
I wouldn't be surprised if your router wasn't having too much runout at this point either. To get best results out of a PC router you should change the factory collet for one made to adapt it to CNC use. They improve it's performance a tremendous amount. Precise bits has one that is used by many and well thought of.

[srwtlc]

Don't know if ArtCam has the option or not, but I'd use a spiral ramp toolpath that spirals down as it cuts around. That would keep more of a constant smooth motion to the cut. With a up spiral cutter, you should be able to do at least .375 per pass. At 26000 rpm, you're going to burn up and dull your cutters quickly. Since it's a PC, try 16000 or less (the lower you can go and still make a quality cut, the better).

If your toolpath is .25 per pass and the machine is cutting .3125 per pass, your unit values might need looking at (particularly the z axis). Or you may have some slippage, lost steps, or gantry flex going on. Gantry flex could also cause chatter on the profile.

Cross posted with Dave.

[donek]

To start with, you need to grab onto that tool/router spindle and see how much play there is. The Z-axis on the PRT can be extremely accurate if it's adjusted right, but if everything is all loose and sloppy it doesn't work well at all. I've replaced the uprights on my PRT Z-axis about three times, but that includes flipping them over and using all four surface before disposing of them. There is actually very little mass to the z-axis on a PRT as well, so vibrations can be a serious problem. After checking the play in the z, you need to check play, backlash and even look to see if the y-car is lifting off the rails when plunging. The PRT is a great machine, but like any it requires the correct maintenance. The simple fact that the unit values are incorrect is a good indication that the machine was not maintained correctly.

The more material you remove with your cutter, the more power it takes. I'd approach this with a smaller diameter cutter, probably 3/8. A typical straight flute cutter can't make a plunge cut because there is not cutting surface at the center of the cutter. With the 1/2in cutter, you're still trying to cut with a portion of the cutter that has no cutting edge. Move to a smaller cutter and spiral into the hole. If you go to a 3/8in plunge cutting spiral bit, you may want to peck drill the hole in the center and then spiral down to get the final dimension. You may actually have to make a roughing pass and then a final pass, removing only 0.030 to 0.050in in order to obtain the results you require.