PDA

View Full Version : Swapped to a 1/2" bit, and everything went wrong... why?



jeffreymcgrew
01-20-2007, 12:20 PM
Hey all, I need some pointers.

We just upgraded our PRT to a 4g. Very, very happy. However, today we tried to cut 3/4" birch plywood with a 1/2" compression spiral, taking 1/2" deep passes at 6 inches per second. Nothing but trouble. I tried several different speeds, and different RPM's on the router, and no luck. I'd still get stalling and even wandering where it appeared that the router was taking over the Shopbot. Not good.

I used values given to me by the Chip Load Calculator, and I tried several slower speeds too. Is a 1/2" bit taking a 1/2" pass just too much to ask of my 'bot (remember, it's not an Alpha, and only has the standard PC router), or am I doing something wrong?

Brady Watson
01-20-2007, 12:57 PM
Jeffrey,
I think that a 1/2" DOC @ 6 IPS is a tall order for a standard PRT. While the 4G upgrade is pretty amazing, keep in mind that they are still about 1/2 the torque of a standard Alpha motor.

You may want to try going .25" per pass and pull that speed down to about 4 or 5 IPS, depending on how convoluted the design is. The goal is not to break the magnetic lock of the steppers while cutting; that's where you lose steps. Going forward, you may find a 1/4" or 3/8" compression better for your tool since each require less cutting force than the 1/2" bit at the same speed & RPM.

-B

jhicks
01-20-2007, 01:07 PM
Hey Jeff, I can tell you that we cut 3/4" 7 ply prefinished birch with a 3/8" compression bit full depth at 160 IPM at 15,000 rpm on a PRT with spindle, G Code, and ascension control box with 1 AMP motors.We can move faster but this seems to be our sweet spot on this material.

I think the move speed of 6IPS or 360IPM is asking more than a PRT can deliver successfully but leave that to those more informed than I.
Tech support at SB can confirm but I think I'm close on this.
As I recall a PRT may not be able to get much past 2.5 to 3 IPS/ 180IPM depending on art files, software, PC, motors, shape, ramps etc.
In our case I think the motors are the limitation on higher speeds now but with sb code it may be the limits on communication to motors.
Of course Alpha and new G4 are more able to move and cut at elevated speeds as well.

jeffreymcgrew
01-20-2007, 03:28 PM
Brady, thanks for the info. We've been getting along just fine with a 1/4" compression spiral @ 6 ips when taking 1/4" passes, so we've just gone back to that. Get more out of a sheet anyways that way, for we can nest things tighter. Just looking to see if we could cut in two passes instead of three.

Jerry: with the 4g upgrade a PRT can go into the 6-8 range if there isn't too much load on the router. We're cutting at 6 ips all day long without trouble when using a 1/4" bit and only taking a 1/4" pass...

jhicks
01-20-2007, 04:12 PM
Understand Jeffrey now that I read you have the G4 upgrade. To each his own but we just felt that 3 passes still leaves variation in edges per pass and single pass leaves no such marks.
Of course if yield is that tight/critical 1/4" is the way to go even if it is more cut time.
In the end, its about the results that satisfy you and your customer

jeffreymcgrew
01-20-2007, 04:39 PM
No, I wish we could do a single pass. That's never seemed to work for us. So what we do is two passes at a 0.020" inch offset, leaving a .125" skin behind, then on the final 'cleanup' pass the bit cuts away that skin and then also 'shaves' the edge clean. With a compression bit we get pretty clean edges this way, and it lets us cut at 6 ips.

Also you've got a Spindle, which I wish we had. We only have a router, so we're limited in how deep we can cut before it starts to bog...

richards
01-20-2007, 05:11 PM
Jeffery,
The numbers from the chipload calculator don't always work with the PC7518. With a spindle, the VFD controller is (usually) able to spin the cutter at the specified RPM's, but the 7518 will bog down. Before I installed my spindle, I normally had to use the three highest speeds on the router to get the torque that I needed.

You might also try cutting with a CLIMB cut except for the final cut and then switch to a CONVENTIONAL cut. Gabe taught me his method, which he describes here (http://www.talkshopbot.com/forum/show.cgi?tpc=29&post=41367#POST41367). It works.