[gixxergary]

Have a little problem with my vf0e mill. Using a mastercam x7 program with dynamic core milling to do a boss on top of a plate. The program runs perfectly in mastercam verify, runs perfectly on the graphics screen on the machine, but yet, at 500 ipm back feedrate, I seem to be getting a dog leg move that is snapping endmills, as the machine cant seem to roll around a corner clearing the remaining stock. This program also runs on my 08 vf4 with no troubles. I found setting 57, exact stop. This was turned off, but its been off for years with no troubles. Going to turn it on in the morning and re-run the program to see if this helps.

Any insight as any other setting or parameter that would need to be changed so it doesnt make this move??? It may be time to upgrade this machine, but its bought and paid for itself many many times over, so would be great if this could be remedied.

Thanks,

[neilw20]

Some pictures would help us assist you. Maybe a snippet of code where the problem is too.

[Machineit]

Have a little problem with my vf0e mill. Using a mastercam x7 program with dynamic core milling to do a boss on top of a plate. The program runs perfectly in mastercam verify, runs perfectly on the graphics screen on the machine, but yet, at 500 ipm back feedrate, I seem to be getting a dog leg move that is snapping endmills, as the machine cant seem to roll around a corner clearing the remaining stock. This program also runs on my 08 vf4 with no troubles. I found setting 57, exact stop. This was turned off, but its been off for years with no troubles. Going to turn it on in the morning and re-run the program to see if this helps.

Any insight as any other setting or parameter that would need to be changed so it doesnt make this move??? It may be time to upgrade this machine, but its bought and paid for itself many many times over, so would be great if this could be remedied.

Thanks,

I think what you are having is a look ahead issue, with not enough block look ahead and memory for the older machine to run at that speed. To me, if you are running a 400 ipm, you need to make changes in the program to more effectively use the endmill/machine.

Mike

[gixxergary]

Mike is right. Ran the program above the part at 250 ipm back feed rate, and it worked correctly. Setting 57 had nothing to do with it apparently. It was the look ahead. This higher speed machining tool path is just too much for the older machine. When we post out to that machine from now on, we will compensate for it.

Thanks for the responses,
Gary

[SBC Cycle]

I have Fadals in addition to Haas VMCs. In the Fadal there is an M-Code setting and a parameter setting that affects the way the tool moves around a sharp corner. M96 is for "corner rolling". When milling a 90 degree corner, for example, instead of moving in two straight, perpendicular lines the tool gets to the edge of the corner and "rolls" around it as if you had programmed a tiny radius on the corner. In M97 mode, the move is always "intersectional". The cutter will overshoot the corner until it is in position for the next linear move, then continues on that path.

Sometimes that will cause a collision if you have another boss that lies in the path of the intersected move. A picture would be helpful here but I don't have time to make one. I think the OP is looking for a setting that would force the tool to "roll" around the corner - staying in contact with the boss he is machining. I haven't found that setting (if it exists) in the Haas.

EDIT: I guess I misunderstood the question and the OP has the answer (very intuitive Mike!). But I would still be interested to know if the Haas has this feature. I have had collisions when running a profile around a very pointy feature and the tool has overshot the corner until it intersects with the next move. I have fixed the issue by putting a tiny radius on my geometry to force the roll.

[fizzissist]

@SBC Cycle..
I seem to recall a G8 on the Fadal that smooths out the cutter movement.... Format 1? I initiated it at each tool change, just in case I had to run from a tool change.

For the Haas, having look ahead really helps. We enabled the option on the VF9 and it made a WORLD of difference. (it should, given the cost)

[SBC Cycle]

We also enabled the High Speed look ahead on our older Haas and it made an immediate improvement in both part quality and tool life. I have a neat photo of some high speed machining "blemishes" that after investigation turned out to be minor fluctuations in the toolpath that showed up in the finish of the part. That's amazing that the Haas duplicated it at the speed I was running. And no corner clipping, it stays right on track. Yes, for the money I was pleased it works pretty much as advertised.

Your memory is correct about the G8 in the Fadal, it also works in Format 2 but it is also touchy about not staying modal. It is described as "No Ramps" so not quite a look ahead feature but definitely smooths a CAM generated toolpath. The G9 is "With Ramps" and although not exactly an In Position Check (Exact Stop) it will act like one.

My corner rounding question above turned out to be un-related to this topic.

[Ydna]

I've dealt with this a bit when running older mills. I've found it's invaluable to use arc tolerance filters with the dynamic toolpaths. The machine can interpolate the G2 or G3 movement better than hashing it up into 20 small G1 moves. However, sometimes the code will overcut on the lead in/out, so you might have to increase the material to leave on walls to a higher number like 0.015".

The Haas setting that controls speed is number 191 ("smoothness"), which allows you to choose between three options. Selecting "rough" will make the machine cut noticeably quicker but the accuracy will suffer. Setting it to "finish" will cause some noticeable slow-downs in corners.
You can also force these options into your programs using "G187 P1" or P2 or P3. It overrides setting 191 while the program is running.
You can also adjust setting 85 "accuracy" but it has more of an effect on accuracy rather than clipping corners and speed.

Unfortunately though, the older machines don't have settings 191 or 85, but if the machine has high speed machining option then it probably has them. I don't know when it was added but my pre-2000 mills don't have it.