mazak high speed machining

[Dakota]

Hi Guys

in high speed dynamic area toolpath should I use G5 P2 (Mazak high speed) in the program or no?

Thanks

[djstedman]

I think this only will work if you have the option MAZACC3D, I believe its Mazak's 3D High Speed Smoothing Option

 

I know if I try and use it I get an alarm.. however I do use G61.1 to enable feeding over 315IPM

 

For what I have done using our newer Mazak's using G61.1 is enough to hold pretty fussy 3d profiles without having that option.

 

If your going to enable high backfeeds (critically important to reduce cycle times) and or feedrates over 315IPM then you will need definitely need to use G61.1

 

Im interested to see what others have to say about this though..

[Hertz]

You don't need to use G61.1

I just change the feed paramter from 8000 to 30000. If you have a good programmer that can control the feeds through Mastercam High Feed option, you don't have to worry. G61.1 sucks in my opinion. It jerks too much. Can't change the acceleration of it afaik besides the K value but it gets to a point when the jerkiness is gone, it ends up way too slow in the corners. Its a weird feature. they ahve the right idea, but needs adjusting I think.

My max feed is 1180 IPM hence why my parameter is set to 30000. You have full control in Mastercam for slowing corners. I prefer it that way but definitely do not HAVE to use G61.1

 

There is one issue though and that is if using conversational, you need to remember that parameter is set high and your operators need to be aware of it if they are writing programs at the machine over those speeds.

[Joe788]

You don't need to use G61.1

I just change the feed paramter from 8000 to 30000. If you have a good programmer that can control the feeds through Mastercam High Feed option, you don't have to worry. G61.1 sucks in my opinion. It jerks too much. Can't change the acceleration of it afaik.

My max feed is 1180 IPM hence why my parameter is set to 30000. You have full control in Mastercam for slowing corners. I prefer it that way but definitely do not HAVE to use G61.1

 

There is one issue though and that is if using conversational, you need to remember that parameter is set high and your operators need to be aware of it if they are writing programs at the machine over those speeds.

 

There are a bunch of parameters for tuning G61.1. I don't remember them off the top of my head, but I think there are a few in the F section and a few in the L section.

[scooke4073]

You don't need to use G61.1

I just change the feed paramter from 8000 to 30000. If you have a good programmer that can control the feeds through Mastercam High Feed option, you don't have to worry. G61.1 sucks in my opinion. It jerks too much. Can't change the acceleration of it afaik besides the K value but it gets to a point when the jerkiness is gone, it ends up way too slow in the corners. Its a weird feature. they ahve the right idea, but needs adjusting I think.

My max feed is 1180 IPM hence why my parameter is set to 30000. You have full control in Mastercam for slowing corners. I prefer it that way but definitely do not HAVE to use G61.1

 

There is one issue though and that is if using conversational, you need to remember that parameter is set high and your operators need to be aware of it if they are writing programs at the machine over those speeds.

 

Whoa!

 

G61.1 is NECESSARY. If you do not run it with dynamic tool paths, you will over cut and break xxxx (trust me) . The reason it is "jerky" is you need to adjust it a bit better. Take a look at parameter L75. There is also L74, F8 and a bunch more. Seems to me that you decided to blame the machine instead of trying to understand it a bit better.

 

Also, G61.1 is on by default in a Mazatrol program....no need to make your operators aware.

[Hertz]

There are a bunch of parameters for tuning G61.1. I don't remember them off the top of my head, but I think there are a few in the F section and a few in the L section.

I was told by Mazak that I just need to change the K value to alter the acceleration/deceleration.

Eg G61.1,K70

Said to make adjustments, change the K value, however like I mentioned above, it still started/stopped too jerky but by the time I was satisfied with the speed, it was just way too slow in corners. Depending on your needs, you may like it, I just found it too rough for my liking.

[Hertz]

I have not used G61.1 since 2007. I use the high feed option in Mastercam. I do a lot of HSM, nothing breaks. Mastercam handles the corners quite well. Actually better than G61.1 in my opinion. So its not necessary per se.

I never blamed the machine. I said i preferred Mastercam control. I actually called Mazak, they never told me about the other parameters AT ALL. So please don't put words in my mouth.

 

Also, G61.1 is on by default in a Mazatrol program....no need to make your operators aware.

Good to know. Never hurts to be safe so I will still make my operators aware.

[scooke4073]

,K is just an accuracy coefficient.

 

Tell me what your L75 is set to.

[scooke4073]

To answer the original question....

 

It's not necessary. G05 P2 enables 500 block look ahead. Mold cavities...Yes. Dynamic area...Not really.

 

Although I typically use it all the time....why not.

[Hertz]

I can't use the G05 P2. Apparently it was not an option the owner wanted. As for the L75, its set to 1000.

[scooke4073]

1000 is pretty high.

 

I'm assuming you have a VCN with Matrix control? I've run L75 as low as 300...however shape accuracy becomes an issue. It takes some fine tuning but you can dial it in to run smooth as silk. High smoothing control is a great option that gives you great control over acceleration/deceleration parameters. If you do a lot of high speed machining, it might be worth a look.

[djstedman]

guess I have been lucky but on our machines with no parameters tweaked at all the g61.1 option runs very smooth up to as high of feedrates as I have found our tools capable of handling..

[Joe788]

I was told by Mazak that I just need to change the K value to alter the acceleration/deceleration.

Eg G61.1,K70

Said to make adjustments, change the K value, however like I mentioned above, it still started/stopped too jerky but by the time I was satisfied with the speed, it was just way too slow in corners. Depending on your needs, you may like it, I just found it too rough for my liking.

 

As others have mentioned, the K value is just the accuracy coefficient. So you can call G61.1,K10 if you want it to round off the corners and go a little faster, or G61.1,K70 (which is default, simply G61.1 will do) to make it cut sharp corners.

 

All of the machine specific tuning is in the parameters. I doubt Mazak expected people to run the VTC250/D the way you guys are running it, so no real engineering time was spent on the fine tuning of the default parameters. I think they expected more of your big 6 inch face mill, and less of the 3/4 endmill at 500ipm.

[Hertz]

As others have mentioned, the K value is just the accuracy coefficient. So you can call G61.1,K10 if you want it to round off the corners and go a little faster, or G61.1,K70 (which is default, simply G61.1 will do) to make it cut sharp corners.

 

All of the machine specific tuning is in the parameters. I doubt Mazak expected people to run the VTC250/D the way you guys are running it, so no real engineering time was spent on the fine tuning of the default parameters. I think they expected more of your big 6 inch face mill, and less of the 3/4 endmill at 500ipm.

 

lol perhaps you are right. Anyway, it is not a Matrix control. Its a Fusion 640M. Machine is a VTC 250D.

So lets say I put the L75 to half. Would it be smoother in the corners?

Right now the K value does indeed slow the toolpath down. I am not sure what I am missing. It seems to me you are telling me the K value only adjusts accuracy. Wouldn't this be a result of slowing down?

If I run G61.1 with default K value, its jerky as hell. I can't keep it like that as it hits pretty hard. What will cutting the L75 value to half actually do?

[Hertz]

guess I have been lucky but on our machines with no parameters tweaked at all the g61.1 option runs very smooth up to as high of feedrates as I have found our tools capable of handling..

 

What kind of feeds are you running though?

[djstedman]

It depends on what i'm doing and cutter diameter, depth of cut etc.. , but in general In a dynamic mill in steel I'm generally cutting around 200+IPM with backfeed set to 1000IPM, in Aluminum I'm pushing more have been as high as 500IPM with the cutting with the backfeed around the same.. 1000IPM

[Joe788]

lol perhaps you are right. Anyway, it is not a Matrix control. Its a Fusion 640M. Machine is a VTC 250D.

So lets say I put the L75 to half. Would it be smoother in the corners?

Right now the K value does indeed slow the toolpath down. I am not sure what I am missing. It seems to me you are telling me the K value only adjusts accuracy. Wouldn't this be a result of slowing down?

If I run G61.1 with default K value, its jerky as hell. I can't keep it like that as it hits pretty hard. What will cutting the L75 value to half actually do?

 

The parameter manual should have a slightly detailed explanation - though I'm not a motion control engineer so a lot of it is greek to me. The K value only adjusts HOW MUCH it slows down, not how violently or smoothly it slows down. That's what the F and L parameters are for. There are different values that are assigned to different rates of direction change, acceleration/deceleration, etc.

[GPC_CNC]

1000 is pretty high.

 

I'm assuming you have a VCN with Matrix control? I've run L75 as low as 300...however shape accuracy becomes an issue. It takes some fine tuning but you can dial it in to run smooth as silk. High smoothing control is a great option that gives you great control over acceleration/deceleration parameters. If you do a lot of high speed machining, it might be worth a look.

 

I've tuned our mazaks L75 to about 300-350 depending on the vintage. High speed smoothing control is fantastic as it gives you several levels of control in the parameters behind G61.1. I've reset level 1 L75 to 300 and mainly keep it there. There are M codes M821-M830 (level 1-10) that can be adjusted on the fly in the program. For almost everything I leave it at level 1 and when I need something to be very precise I'll change the level to suit. Without G61.1, the machine cuts corner like a xxxx unless you baby it.

 

Greg

 

Also, to be more specific L75 controls accel/decel as a line enters another line (or arc) at a tight angle. In other words the lower the value (in milliseconds) the later it will decel into a corner and the earlier it'll accel out of a corner. You will see less slowing down on arc moves, but the machine will jerk a bit more. We haven't seen any adverse affects from this yet, not to say there won't be. You can always opt to not use G61.1 and the machine won't jerk around, but that's because it's cutting off you're corners and you won't be able to feed above 315ipm. Factory settings of G61.1 don't seem very performance oriented and require user tuning.

[Hertz]

I've tuned our mazaks L75 to about 300-350 depending on the vintage. High speed smoothing control is fantastic as it gives you several levels of control in the parameters behind G61.1. I've reset level 1 L75 to 300 and mainly keep it there. There are M codes M821-M830 (level 1-10) that can be adjusted on the fly in the program. For almost everything I leave it at level 1 and when I need something to be very precise I'll change the level to suit. Without G61.1, the machine cuts corner like a xxxx unless you baby it.

 

Greg

 

It may cut like xxxx if you don't use anything. I use the Mastercam High Feed option to control corners. It works fine. That was my main point about not HAVING to use G61.1. There are other methods. I'm going to try to adjust the L75 parameter and see how it changes. Thanks.

 

**EDIT**

I ran a sample program with the G61.1 on with the default K value of 70 and the L75 parameter at 1000. As suspected it was too slow to get to speed, however the machine was still jerky. Perhaps its cause of too many X and Y moves in the program? I changed it to 300 and re ran the program. I had to stop it cause it sounded like it was going to take off running it was jerking so bad. Seems I would have to go higher to smoothen out the jerkiness. Its already high as it is and never has time to reach optimal speeds. Seems Mastercam does a better job for me for the HSM. I'm not sure what other parameters I should look at or play with to get it right so I'm going to stick with Mastercam's high feed options. Produces more code, however it runs a lot smoother.

FWIW - default on the L75 parameter on this machine is 1000.

 

Also one more thing to the OP. Sorry for hijacking your thread.

[PcRobotic]

G61.1 (MAZAK HIGH SPEED MODE ON)
GXX.X (MAZAKE HIGH SPEED OFF)?????

 

I am also looking for the HIGH SPEED OFF code, would you guys help me out the end code?

 

Thank you

[JParis]

G64

 

It's right in the book

[10LIONS]

not sure if you've figured it out yet but I dealt with the same circumstances,

final answer, In- House (Alex Dales) removed the G5 P2 from being output at all in our programs and

Jason Sturgis Mazak Apps, helped me to dial in the L parameters very quickly (he knew his stuff) for G61.1 for our particular machine, 

the machine runs like it should now, also if I run without G61.1, the toolpaths will violate every time, G61.1 is needed for our machine.

hope this helps 

(T2     - 1" HELICAL .03R-4.125" LOC - DIA 1."    - CORNER RAD .03)
T2 M06
T3
G00 G17 G90 G54
M08
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
G68.2 X0. Y0. Z0. I0. J270. K0.
G53.1 P2
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
S12000 M03
X8.758 Y7.023
G43 H#3020 Z6.
G61.1 xxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxx (no G5 P2, also no K value)
Z1.534
Z-1.569
G01 G94 Z-1.594 F300.

[JParis]

1 minute ago, 10LIONS said:

not sure if you've figured it out yet but I dealt with the same circumstances,

final answer, In- House (Alex Dales) removed the G5 P2 from being output at all in our programs and

Jason Sturgis Mazak Apps, helped me to dial in the L parameters very quickly (he knew his stuff) for G61.1 for our particular machine, 

the machine runs like it should now, also if I run without G61.1, the toolpaths will violate every time, G61.1 is needed for our machine.

hope this helps 

(T2     - 1" HELICAL .03R-4.125" LOC - DIA 1."    - CORNER RAD .03)
T2 M06
T3
G00 G17 G90 G54
M08
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
G68.2 X0. Y0. Z0. I0. J270. K0.
G53.1 P2
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
S12000 M03
X8.758 Y7.023
G43 H#3020 Z6.
G61.1 xxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxx (no G5 P2, also no K value)
Z1.534
Z-1.569
G01 G94 Z-1.594 F300.

Not to poo poo on your kind sharing of info....

What you are stating is right for you..perhaps not others...

We run G61.1 with K and R values depending on control vintage....we can run without it as well. We find it most helpful when a corner rad and tool rad are very close to size with each other...

G5P2 is valid on controls that have the option

[10LIONS]

easy JParis,

that's why I stayed specific to our machine and what worked for us big guy