How to adjust accel/decel/corner rates?

[laka]

Recently got a new (to me) 1998 Arrow 1000 A2100

Does anyone know how I can play with the way it slows down etc for corners? At anything over 70 inches feedrate I am losing quite a bit of accuracy on inside and outside corners/rad's.

Thanks

[greg b]

Can you put your feed rates next to your g3 and g2 direct and the back to the faster feed rates when going back to g1 thats what I have done on my Bridgeport and about to try the same on my Arrow.
G1 x110 y0 f300
G2 x 120 y-20 p10 f100
G1 x120 y-50 f300
Dont know if this is what your kooking for,I think theres also a g code that does this to in the book somewere but I cant remember where.Hope this is of some use.

[coop31]

punch in "g45.2" in mdi to see if you have the option turned on. If you do, just put the same g code at the beginning of your program.

Hope this helps.

[laka]

Ya, no go with the G45.2... I was hoping there was some settings somewhere where I could make some adjustments.

[coop31]

You can purchase the option. I think its about $2000. I'm in the same boat.

[maver1ck]

Even if you didn't purchase the die/mold option, you can still adjust the parameters.

I don't have the full list with me, but I believe it is Step Velocity, Feed Max accel, Jerk Value, VFF% and Collinear Angle that were adjusted.

In earlier versions of the control, you had to make the changes to each axis individually, later versions created a common page so most of the adjustments could be made on a single page.

[laka]

Thanks for that info Maverick. I did see that page, and assumed it would help me out, so now I'll play around with it and see how she goes!

[laka]

Hmmm. I tried playing with these numbers.. a lot. And no noticable difference. I cut the numbers in half, and in half again and restarted the machine and everything still looks the same when I cut my piece. Any chance you would have that list handy maverick?

[greg b]

Im not sure those values talked about are going to make the change you need,I know jerk value is how quick the machine changes direction and if you ajust it its going to change every thing in the program not just the corners,where the g45 is a look ahead type function that the control automatically computes a smoother transition along its path and will work out its own feed rates for each position.I wasnt aware that was a pay for option,I must try that tomorrow I guess that would be in the paid for options field in the control.

[maver1ck]

I'm not sure which software version you have, but since you mentioned finding a single page with those values, I'm guessing some version of Release 3.

On this version of software, there were two options for Die/Mould machining, a standard which included a faster processor and some parameter changes, and enhanced, which also included the selectable Acc/Dec (G45.2, etc.). Without the selectable acc/dec, you can still use these settings, they just have to be manually entered into the table each time you want to change the machining mode.

If you look under Axes/Servo on the Process rates tab, you will see the basic settings for G45, G45.1 and G45.2. If you want to see how these will affect machine performance, try taking the G45.2 values and putting them into the G45 row in the table. Jog the machine using the hand pendant, and you should notice the moves are substantially softer as the machine accels/decels. This may be too slow for what you are trying to accomplish, but you can work back up from these values toward the original until you find a combination that works for you.

If you enable VFF, you will also need to set a VFF% in the Feedforward Parameters (under the Servo Tuning page). What this should be depends on the machine, but for your 1000 start with 95%. Each Axis will need to have this set individually.

[laka]

I have version 2.34 software on my machine.

I couldn't locate the Process Rates tab you mentioned. I did find 'Axis Rates' under the Axis button in System Configuration. I have tried adjusting the Step Velocity and Accel Rate numbers on my X and Y axis, with not much luck. Any chance I could get some values from your machine to cross reference? Some of the numbers in my control look very high.

Also, my machine shows no reference to G45, G45.1 etc anywhere in my System Configuration. G45 is enabled on my machine, but G45.1 etc does not work. Should this table for G45 etc be on my control somewhere? I feel as though I have missed a screen somewhere but I know I have been through everything. I am using the 'worldclass' password.

So far regardless of what I have done, I am still having less than desirable results on running high feedrates and over/undercutting corners. Thanks for all the help so far guys!

[maver1ck]

Don't actually have a machine to give you values from, doing this all from memory.

The previous info was for Release 3 software, since you have release 2, changes things a bit. Instead of Process rates, you will need to look at the Axis Rates page and change the X,Y, and Z values individually.
Lower step velocity to about 20% of original value
Lower accel rate to about 50% of original value
Multiply reversal threshold by 10
Set VFF Gain to 65 (VFF also needs to be set in C)

Then go to the path data page and set
Lower Feed Max Accel to about 3% of original
Lower Jerk value to about 8% of original

Also, since this is a new to you machine, have you checked for mechanical issues? No matter how much tuning you do to mask an accuracy problem, if the thrust bearings or ballscrew are bad, you are still going to have problems.