How to Smooth machine motion

[Chris Flint Two Ft Pty Ltd]

I have just completed a long program where the CNC has to constantly interpolate all 3 axis.

I find that V9 tells me it will take 6 hours to machine.

I send it to the machine and run it it takes around 9 hours.

When the motion (up and down ) is happening the feed speed is constantly adjusted , I presume by the controller.

The motion is therefore very jerky and I think I would like some way to smooth the whole thing down.

Highfeed, just seems to add about 40% more time to the machining cycle.

Surely MC is supposed to cater for the up and down movements, or is it just a slow controller problem.

Is there another way.

thanks in advance

chris f

V9 Mill 3 with ART

[Greg Williams]

Chris,

 

This sounds like a controllerMachine problem,

 

Essentially either the controller cannot read the blocks fast enough or it cannot store enough blocks in the buffer (could be the transfer Baud rate if using DNC), or the axis encoders cannot adjust fast enough to maintain the feed rate.

 

I believe that your problem has little to do with mastercam and more to do with the machine, My only suggestion is use the filter at 3:1 setting and try to program within the arc planes.

[Chris Flint Two Ft Pty Ltd]

Budgie,

where is the filter setting you are speaking of, the relief is being machined under art and I am not sure I have seen a setting as per the 3:1 you speak of??

chris

[smokey_44]

Budgie ...I think your right on the money with that ,cause we used to run cmm scan data programs with very small xyz moves and it was the exact problem , only way to fix it is to filter the program to remove some of those points ....or get a larger buffer for the machine $$$$$$$

 

 

Dave

[lynnz]

the 2:1 filter setting is what I use with good results. I think it is the recommended setting.

 

Try that and see if that helps.

 

lynnz

[gti_jay]

Does your machine have a "highfeed" mode?

 

it may be called GI or SGI or something fancy like that...

 

The cause is the machine accel and decel.

 

Mastercam simply measures the length of cut and multiplies it by the feed rate. Voila. Cycle time.

 

It cannot possibly accomodate different acceleration and deceleration parameters of different machines and programs.

 

I know it sounds bizzare and wrong, but you may have some success by actually slowing down the programmed feedrate to find the "sweet spot" in your machines accel/decel limits.

[toolall1]

was the 3:1 filter a typo or is set custom?

i dont see it either .

thank you

[jbert]

go to parameters tab/ total tolerance.

be sure to program paralell to x or y.

[jbert]

my total tol shows

off

1:1

2:1

3:1

custom

[within a thou]

removing block numbers and whitespaces will help to you can also look at haing a second post made that only outputs up to 3 decimal places to reduce block sizes

[Müřlıń®]

quote:

---

Highfeed, just seems to add about 40% more time to the machining cycle.

---

Yes most of the time it does for that type of app.

 

 

Others would disagree with me, but Highfeed should be used to add acel/decel when your control wont do it.

 

On a very long program, operators will tend to override the feedrate down to the min it takes to run the program so they don't have to sit on the override pot like a gas pedal.

 

Running the highfeed filter will actually make your programs run faster.

 

You have to experiment with the settings to get a happy medium in fluent motion....

 

I use the Highfeed filter on every job.

[toolall1]

o.k thanks

its there

thank again

[Yogesh K. Raman]

Mastercam Art only has tolerance for Cut tolerance with no ratio setting, at least I can't find it...

[Chris Flint Two Ft Pty Ltd]

Sorry I dissapeared for a day, We do not have a filter tab that is settable in ratio in MCART I know it is there in Mill 3 surface toolpaths.

As far as buffer is concerned, I am drip feedin the machine and it has a buffer of 35000K which I am sure is a enough in that I can watch the PC that is sending the data stopping and starting in order to replenish the buffer and it appears to not have any effect of the smoothness and the CNC is certainly not waiting for info.

As far as highfeed in the controller is concerned I do not know and will check with the controller supplier.

I cannot use block numbers in that the control has a limitation of N99999 and then tries to go back to N1 so ""CRAAAASH"" so as a matter of course I have the post set to not produce numbers or spaces, most of the file sizes i run are 3 Megabytes or around 300000 lines of code.

Merlin,

I think you are right, I will certainly try to use highfeed and see if this assists.

thanks all

chris flint

[majariley]

chris, our fadal controllers use a g8 to turn accel. and a g9 to turn on decell. we always add the g8 to the start of our program and it really makes a difference.