Jerky Fadal

[KJS]

When we mill an arc with our Fadal VMC, it seems to jerk alot. Almost as if it pauses after each line before making the next move. This only occurs when doing arcs, other movements seem fine. Thanks in advance for any help.

[steve f]

If you're drip feeding, the baud rate is probably too low.

 

steve

[Tim Johnson]

We had the same problem with our 6030. We would get jerking with out tapping also. Fadal's solution was to turn off our scales. The jerking did stop but now we tolerance problems.

 

FADAL SUCKS

[EX-wccprogrammer]

Fadals have an Acceleration mode that checks the position before the next block is executed. G8 forces a pause for position check, G9 disables it. Try inserting a G9 in the program.

[cadcam]

Insert the G8 not the G9 and this will help.

[ssibiski]

I thought G9 enables position check( which would cause the jerk motion) and G8 disables it so it doesn't ramp down the Feed though corners. I might be wrong though.

 

Steve S.

[Tim Johnson]

Actually G9 decelerates the control. To enable position check you need a second G9. If you are already using G9/G8, try turning off the scales.

FADAL was in here three days trying to figure why our 6030 was jerking. Every once in a while during tapping it would vibrate so badly the machine would physically move.

[crazy^millman]

I always use G8 for our 3d toolpaths and never have a problem. I would check my coupling at eac haxis and make sure there is no play in them. The x is easy the y is harder. Take off the cover and grab the coupling and see if there is any slop in the motor shaft to the axis shaft if there is I would have these repalced as soo nas possible. Hard to hold something right if there is alot of slop here. If you use all the above ideas and still have trouble then I would check to make sure you have arc for maves and not point to point moves for the arc moves. Write a simple G2 or G3 move ot make a 6" cicrle and cut it in an aluminum plate. I would make the hole a finished sixe to shot for. I would then check the hole in 16 places like around a clock if you get more than .001 then you have got problem with your machine adjustign the backlash correctly and need to get the machine serviced.

 

Just my opinion and that it and use it however you want but do so with caution.

[EX-wccprogrammer]

Sorry, guys... I had the codes backwards, have not used Fadal for 3 years.

[crazy^millman]

No problem you were trying to help and to some of us that counts but to others if you are wrong you can be burned at the stake but me I appericate effort and trying to get something going. I see it time and time again guys just kind of go well if maybe or do this or might do that but never give a direction and even if the wrong start good to get to the right place and seem like always hardest to get the balling rolling verse pointing it in the right direction. I appercaite the effort and always feel free to help.

[Barghest]

If you have a DC machine I would check my resolvers. And if you have an AC machine it could be your encoder. Loose couplings and high feed rates i have seen to cause this also.

[John T.]

If you are cutting a 2D arc, check if the arc is a nurbs spline instead of an arc. If so, replace it with an arc. That alone should smooth it out. If for some reason you can't do that, use a G8. You can do that automatically by clicking on the operation, parameters, misc values, and on the 4th line, should say acceleration/decelaration. 0 is G9, 1 is G8.

All surface (3D) operations get a G8.

John

[crazy^millman]

John T since we mainly do 3d work our post is hard coded with the G8 to post out automatically and it does not give us any probelm when we do Drilling or 2d work or even rigid tapping on the machien that has wit hthe Fadals.

[cadcam]

(You can do that automatically by clicking on the operation, parameters, misc values, and on the 4th line, should say acceleration/decelaration. 0 is G9, 1 is G8. )

 

Jhon T , only if your post is set this way .

Not all the fadal posts have this option.

[Thad]

Ron, Fadal actually recommends a G8 with rigid tapping. It's supposed to make the reversal at the finish depth smoother.

 

My guess would be that you're not cutting arcs, your cutting splines or tiny line segments.

 

Thad

[crazy^millman]

Yeah kind of what I thought when I just hard coded the post that way. I also liek the fact that you are not slamming the machine all the time either when making moves over 200 ipm.

[John T.]

Ron,

Unfortunately, our post isn't set up to automatically put in the G8's. Since I'm not the guy "in charge" of MC where I work, not much I can do about it, even if I did understand the post language enough to change it. If I did understand it and knew what to change, then I'd suggest it. It would probably be accepted cause the shop boss is on an efficency kick.

 

John

[MetalMarvels]

I have also seen this before when cutting an arc that is "rotated" from the normal 0 - 90 - 180 - 270 break positions. I think that I changed "breakarcs" to break at quadrants to fix it.

[KJS]

Thanks for all the help. I will try it asap. I'm kind of bogged down on other projects right now.

[billystein]

try post fad9.pst. make sure you download fad9.txt. Set misc int 2 to 1 to enable g8 in contouring

[Trevor Bailey]

I have a fadal post that will reconize the operation type and insert the G8/G9 code respectively automatically. There is never a need to turn anything on. Let me know if you would like it and I will send it to your dealer.

[Thad]

Trevor, how easy would it be to incorporate just that feature into an existing post?

 

Will it give rigid tapping a G8 or G9?

 

Is it for format 1 or 2?

 

Thad

[Steve Biehl - Cimquest Inc]

should be pretty easy to do. I mentioned in another thread about setting 'getnextop : 1' in post. You can then check in psof/ptlchg the value of 'nextdc'. Zero or greater means the next op is drilling. Something like this.

code:

---

psof

...

if nextdc < 0, #milling cycle

[

pbld, n, "G8", e

g8g9_flag = 1

]

else,

[

if g8g9_flag = 1,

[

pbld, n, "G9", e

]

g8g9_flag = 0

]

...

---

Put something like this in the psof/ptlchg/ptlchg0 sections.

 

I'd also use the flag to know to put out the 'G9' in the pretract section just before a toolchange.

[billystein]

Try bfad9.pst from the ftp. make sure you also get the bfad9.txt file. It also has the cool tool list from one of the newer posts.

There is a mc9 file called posttest. I made it to test some important features that you don't think about.