Trouble with Multiple Retracts on Peck drill cycles

[Zagadka60]

Hi, I'm a little new to all this, so if my terminology or placement is stupid, let me know.

I work on a Haas mini mill, using NX7.5 to make my code. all the parts i make are fairly irregular bodies, single part, double sided. One of the things i always need is a hole array in the part, usually offset from the edges by a bit, and so on. i've figured out how to set up the holes specifically in the part, and assign them to be cut, but currently, my machine only reads the first retract plane and ignores the rest, leading to it crashing. i've got a few solutions for this, none of which are particularly elegant. I'm wondering if there's a mill setting to recognize additional retract planes, or, alternately, if i need to rewrite my post.

Thanks in advance!

[mactec54]

Zagadka60

Post the code you are trying to use, we will have a better idea of what may be happening, G83 or G73 work fine on the Haas machines

[Geof]

You need to check that your CAM output has G98 Initial Point Return, not G99 R Plane Return and also make sure it has not included a move close to the surface just before the drill cycle.

[Zagadka60]

Here's some of the code i've been using, as far as i can tell, it looks appropriate to what you're saying, but i'm not certain now. I'm thinking maybe my post has some problems on this front.

G40 G17 G90 G70
T07 M06
M01
G1 X4.3448 Y2.5955 F200. S5500 M03
G43 G0 Z-.4133 H07
G83 Z-.8901 R-.4133 F30. Q.0197
G83 X3.6312 Y2.2628 Z-.5137 R-.0503 Q.0197
G83 X2.9175 Y1.93 Z-.3317 R-.0018 Q.0197
G83 X2.2039 Y1.5972 Z-.6642 R-.2381 Q.0197
G83 X1.4903 Y1.2645 Z-.9671 R-.5757 Q.0197
G83 X1.1575 Y1.9781 Z-.9518 R-.5255 Q.0197
G83 X1.8711 Y2.3108 Z-.6142 R-.1897 Q.0197
G83 X2.5848 Y2.6436 Z-.4385 R-.0224 Q.0197
G83 X3.2984 Y2.9764 Z-.747 R-.1662 Q.0197
G83 X2.252 Y3.3572 Z-.8812 R-.3656 Q.0197
G83 X1.5384 Y3.0245 Z-.9807 R-.4105 Q.0197
G83 X.8247 Y2.6917 Z-1.1633 R-.6297 Q.0197
G80
M05
G28

It seems to ignore the R call after the first one. in this case, the move after the first hole crashed into the part.

Thanks for your replies.

[Al_The_Man]

Not sure if this helps in this case, but something that may prove useful at some time.
Al.

[Zagadka60]

That's close, but i don't have a regular enough surface to get a regular formula out of it. thanks though! If i'm reading that right, it lets you mathematically progress through the holes, and i'm mostly working with surfaced facet bodies. if i'm reading that completely wrong, let me know.

[mactec54]

Zagadka60

You Have to have in this case a G99 to actervate the R value
So you need it to be G83G99-------

A G98 does not use the R set value It will return the Z to it's set hight in the program which you dont have one you have all negitive Z settings & R values so need a G99

[Zagadka60]

Brilliant! that's exactly what i was looking for, Mactec54, you're wonderful. thanks a million.

[sinha_nsit]

Originally Posted by Zagadka60 ... G1 X4.3448 Y2.5955 F200. S5500 M03 G43 G0 Z-.4133 H07 G83 Z-.8901 R-.4133 F30. Q.0197 G83 X3.6312 Y2.2628 Z-.5137 R-.0503 Q.0197 G83 X2.9175 Y1.93 Z-.3317 R-.0018 Q.0197 ...

Logically, R-point should lie below the initial tool level (Z-position).
Therefore, change Z-.4133 to, say, Z.05 (I am assuming that Z0 lies on the top surface of the workpiece).
Moreover, if the R-point in below the top surface, you need to retract up to initial tool level (use G98).

[mactec54]

sinha_nsit

I think you miss understand what Zagadka60 is trying to do

Each R value is clearance too the next hole, So to actervate the R he needs to use a G99

His hole starting points are at different heights

He could do with a seperate G0Z3. at the end of the program, the G28 could move all 3 axes at the same time & he could crash into something before the tool is clear

[sinha_nsit]

I thought Haas is nearly same as Fanuc. So, what I said may not apply on Haas.
Moreover, I have possibly not clearly understood what Zagadka60 is trying to do.

[angelw]

Originally Posted by sinha_nsit I thought Haas is nearly same as Fanuc. So, what I said may not apply on Haas. Moreover, I have possibly not clearly understood what Zagadka60 is trying to do.

Hi Sinha,

You're correct in that the HAAS G83 cycle is nearly the same as the Fanuc cycle, but with a few more features. The HAAS G83 cycle also has the following features that are not available in the Fanuc equivalent

I Size of first peck depth (if Q is not used)
J Amount reducing each peck after first peck depth (if Q is not used)
K Minimum peck depth (if Q is not used)
P Dwell time at Z-depth

HAAS also has a setting (setting 52) that allows a distance to be set above the R plane for the tool to retract to after each peck. This allows the R plane to be set close to the work surface, yet has the drill retract well clear of the hole for better swarf evacuation. The difference being is that the drill will Rapid from the Initial Level to the R plane set close to the work surface, thus not cutting a lot of fresh air, but when it retracts after each peck, it does so to whatever value is set in Setting 52 above the R plane.

G98 and G99 work in the same way as the Facuc control. Both are model G codes, with G98 being the default.

What you stated in your penultimate post would have worked, particularly with a an irregular surface. Setting an initial level above the highest point of the irregular surface, and using G98 would ensure that the tool would clear any obstacle when moving between holes, and the individual R planes could be included in each hole definition so that excessive air cutting did not occur.

Effectively, the OP has an initial level that is lower than most of the R planes. Because he initially omitted both G98 and G99, the default G98 would have forced the tool to return to Z-0.4133 before moving to the next hole location. Given that the initial level is lower than all bar 3 of the Zagadka60's R plane coordinates, and his comments in the original post regarding crashing, the drill must still be below the top surface of at least some of the holes. In my opinion using G99 as a fix is a bit of a Fudge, and your suggestion is the more appropriate and elegant resolve.


Regards,

Bill