Need help on my VF2!

[mdn]

I have had a problem when running surface mill on my VF2

When I reduced the tolerance of the program to very small the machine caused a big vibration that I can feel by putting my hands on the front door!

If I let the machine running with normal tolerance the vibration turn into small signs.

Does anyone know the reason causing this situation?

Please help me!

Tks a lot!

[HuFlungDung]

You may need to turn on or purchase the high speed machining option. I think the problem is that the control is not processing enough blocks at the commanded feedrate, so the servos have time to stop while the control catches up with processing.

[mdn]

Tks!

According to your suggestion that I need to buy the HIGH SPEED MACHINING OPTION FROM HAAS then I could see the machine running better with small tolerance! Is it right?

Regards!

[Geof]

Here is some information from the Haas Mill Manual about two settings and a G code that may smooth the machine travel when you are dealing with many small moves. High Speed Machining is only helpful when the direction of travel changes quickly with many sharp corners.

G187 Setting the Smoothness Level (Group 00)
G-187 is an accuraccy command that can set and control both the smoothness and max corner rounding value
when cutting a part. The format for using G187 is G187 Pn Ennnn.
P Controls the smoothness level, P1(rough), P2(medium), or P3(finish).
E Sets the max corner rounding value, temporarily overriding Setting 85 "Max Corner Rounding".

Setting 191 sets the default smoothness to the user specified "rough," "medium," or "finish" when G187 is not
active. The "medium" setting is the factory default setting. NOTE: Changing setting 191 to "Finish" will take longer
to machine a part. Use this setting only when needed for the best finish.

G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness but
leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves
smoothness at its current value. G187 by itself cancles the E value and sets smoothness to the default smoothness
specified by Setting 191. G187 will be cancelled whenever "Reset" is pressed, M30 or M02 is executed, the
end of program is reached, or E-stop is pressed.


85 Max Corner Rounding
This setting defines the machining accuracy of rounded corners within a selected tolerance. The initial default value
is 0.025 inch (except on VF-5 trunion). If this setting is zero (0), the control acts as if an exact stop is commanded
in each motion block.

G187 can be used in the program to alter the effective value of Setting 85, without changing the setting.

[big_mak]

Just for laughs try to turn your feed rate down 50% ans see if it smoothes things out.

HSM is not a cure all if you have more that 80 blocks for a small movement, the machine still may dwell and cause the marks if you feed to fast. You will have to find the happy medium between how fast you will feed, and how fine you set your tolerances in your CAM system.

I just ran a form for Carbon Fibre Layup, and I have HSM, and first one looked like poop, then I droped the feedrate 50% for finishing and it was night and day different.

[Vega Bill]

Hi all,

There is another solution and even for the HSM package. We have been working
with the Haas systems to benchmark the block processing time. While the HSM
package does bring significant improvement to the process time, we have further
reduced the process time and smoothed out the machine motion by DATA-Optimization.

This process embeds acceleration/deceleration into the part program based on the block processing ability of the CNC. We have installed several seats at the GM technical center in Warren Michigan. There the machines are on the second floor of the building and the machine motion got violent enough to shake the lighting fixtures on the floor below.

After the DATA-Optimization was installed, they were able to double the feedrates in the program, produce a higher quality surface finish, and the people working below the machines thought that the equipment had been relocated.

Not only does DATA-Optimization take care of the look ahead, hard corners, and tight radius for contouring, it also takes into account closely spaced data points and reduces the feedrate so there is NO data starvation.

There is a fully functional demo posted at www.vegacnc.com on the downloads page. The demo will allow you to optimize 45 of your own files to prove out the concept before expiring.

Hope this helps 8=)

[big_mak]

I've been booted from other forums for much softer sells!!!!

[MikeOD]

Originally Posted by Geof Here is some information from the Haas Mill Manual about two settings and a G code that may smooth the machine travel when you are dealing with many small moves. High Speed Machining is only helpful when the direction of travel changes quickly with many sharp corners. G187 Setting the Smoothness Level (Group 00) G-187 is an accuraccy command that can set and control both the smoothness and max corner rounding value when cutting a part. The format for using G187 is G187 Pn Ennnn. P Controls the smoothness level, P1(rough), P2(medium), or P3(finish). E Sets the max corner rounding value, temporarily overriding Setting 85 "Max Corner Rounding". Setting 191 sets the default smoothness to the user specified "rough," "medium," or "finish" when G187 is not active. The "medium" setting is the factory default setting. NOTE: Changing setting 191 to "Finish" will take longer to machine a part. Use this setting only when needed for the best finish. G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness but leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves smoothness at its current value. G187 by itself cancles the E value and sets smoothness to the default smoothness specified by Setting 191. G187 will be cancelled whenever "Reset" is pressed, M30 or M02 is executed, the end of program is reached, or E-stop is pressed. 85 Max Corner Rounding This setting defines the machining accuracy of rounded corners within a selected tolerance. The initial default value is 0.025 inch (except on VF-5 trunion). If this setting is zero (0), the control acts as if an exact stop is commanded in each motion block. G187 can be used in the program to alter the effective value of Setting 85, without changing the setting.

Hi,

I just want to clarify something about how setting 191 and 85 work together as well as the P and E calls on G187.

When G187 P1 is called (or setting 191 is set to rough), the E value (or the value in setting 85 if using no E value) is multiplied by 4, and in turn, P3/Finish divides it by 4. This can be very important to know to help avoid stalling around corners. Generally a surfacing program will have enough lines of code that the E value or setting 85 value can become insignificant, but if you don't use the G187 call carefully (and leave setting 191 and 85 at their factory defaults) you can wind up causing some strange cuts and other strange issues.

For typical general part programs I find most people don't bother manipulating the settings or using G187. I actually prefer to never manipulate the settings, I always put appropriate G187 P and E codes into my programs at the appropriate tool changes.

Calling G187 again without a P or E will restore the machine to work from the settings. It will not change the settings, just how the machine will function for the duration of the program you're running.

If you are not sure if the HSM option will be the solution to your stuttering/stumbling with the machine, try it. Most newer machines have the processing power built in, and have HSM available as a trial option. To do this, go to setting 7 (Parameter Lock) and turn it off, pop in the e-stop. Then go to Parameter 315 and set the High Speed Machining bit to a 1. It will generally say 0T (T meaning you have a 200 hour trial). When you set it to 1, it will actually set to 1T, at the end of 200 hours of machine time, it will no longer be available as a trial. So after you try it, if you don't think it helped, set it to a 0 again as you may find another reason to want to try it in the future.

[wms]

Vegacnc,

There is a fully functional demo posted at www.vegacnc.com on the downloads page. The demo will allow you to optimize 45 of your own files to prove out the concept before expiring.

Any way to set the demo to Imperial instead of Metric??