5 axis drilling error

[Rocketmachinist]

So i tired to do some simple 5 axis drilling and came across another error. The tool is drilling at A90. and the first hole comes out fine. Then the b axis should rotate and drill again. But the post is making the A axis go to A-90 and in the process trying to crash through my tools. I thought this post was setup to not go in a -A direction but I guess I'm wrong. Any help would be awesome. I'm on the Haas VF-TR Series 5 axis Trunnion Mill post.

 

N4 M11

N5 M13

N6 T10 M6

N7 G0 G54 G90 X0. Y-6.195 B210. A90. S10000 M3

N8 M10

N9 M12

N10 G43 H10 Z2.7205 M8

N11 G83 G99 Z.2189 R.9705 Q.03 F7.2

N12 M11

N13 M13

N14 Y6.195 B150. A-90.

N15 M10

N16 M12

N17 M11

N18 M13

N19 Y-6.195 B90. A90.

N20 M10

N21 M12

N22 G80

N23 M9

N24 M5

N25 G0 G28 G91 Z0.

N26 M30

[Rocketmachinist]

Also the canned cycle should have a g98 code vs a g99 because otherwise it will crash though my part while rotating.

[Rocketmachinist]

Bump, its an old one but I still havn't had it fixed. I worked with my reseller and got this code out of it.

 

N1 G20

N2 G0 G17 G40 G49 G80 G90

N3 G0 G28 G91 Z0.

( NO. 68 DRILL |TOOL - 10|DIA. OFF. - 10|LEN. - 10|TOOL DIA. - .031)

(HAAS VF - TR SERIES 5 AXIS TRUNN)

(MACHINE GROUP-2)

N4 M11

N5 M13

N6 T10 M6

N7 G0 G54 G90 X0. Y-6.195 B210. A90. S10000 M3

N8 M10

N9 M12

N10 G43 H10 Z2.7205 M8

N11 G83 G98 Z.2189 R.9705 Q.03 F6.

N12 G80

N13 Z4.7205

N14 Z2.7205 B330.

N15 G83 G98 Z.2189 R.9705 Q.03 F4.14

N16 G80

N17 Z4.7205

N18 Z2.7205 B450.

N19 G83 G98 Z.2189 R.9705 Q.03 F4.14

N20 G80

N21 M9

N22 M5

N23 G0 G28 G91 Z0.

N24 M30

%

 

I don't get the z going up to z4.7205 and then moving 2 inches lower and simultaneously rotating the b axis. I would understand it if looked like

Z4.2705'

B.450;

Z2.7205

 

Also why does it change my feed rate from F6. to F4.14?

[Jim at Gentex]

Sounds to me like your clearence plane is set at 4.7205 and your retract plane is 2.7205

There is a check box in the collision control parameters page "Use clearence only at start and end of operation"

I always leave that unchecked.

Also look at whether those are absolute or incremental values.

 

Also in the 'additional settings' > 'misc. values' menu there should be a 'transition retract' and a 'force retract drill 5ax' setting. You may have one or both of those turned off.

 

The feedrate change is probably the default for that tool.

Is the tool listed more than once in the ops manager?

I know that will mess it up.

 

It's a learning process...

[K2csq7]

clear_stck   : 0.    #Add inc. offset to stock definition for transition boundary
retract_on_rpd : 1   #This control allows retract on rapids too (don't assume rapid is safe)

 

 

Found those in the Hass post, the calls for them are in the psb (not found in the pst), so I can't tell exactly what they do...

 

If those don't help..... I would look here. After double checking the linking params...

 

 

prapidout   	#Output to NC of linear movement - rapid           	
     pcan1, pbld, n$, `sgcode, sgplane, sgabsinc, pccdia,
       xout, yout, zout, p_out, s_out, strcantext, scoolant, e$ 	<<<<<<<<<<<<<try changing this line to "xout, yout, zout, e$ p_out, s_out, strcantext, scoolant, e{:content:}quot;

 

 

If you get unwanted breakups of rapid moves in the future, you will need to think up a conditional statement to control when they get broken up.

 

Ad for the feed changing on you....Hrmmmm the obvious would be if you had separate ops for each hole and you just didn't give the other ops the right feedrate..... The 4.14, do you see that anywhere in the tool def?

[Rocketmachinist]

Right now it is one op, (5axis drilling) so everything is incremental no absolute. So it changing the feedrate seems weird to me.

[K2csq7]

+1.....

Do you know anything about "watches" in the debugger? I don't, but it seems like it could be useful to put a "watch" on the feed and see where it's getting changed.....

[kccadcam]

So i tired to do some simple 5 axis drilling and came across another error. The tool is drilling at A90. and the first hole comes out fine. Then the b axis should rotate and drill again. But the post is making the A axis go to A-90 and in the process trying to crash through my tools. I thought this post was setup to not go in a -A direction but I guess I'm wrong. Any help would be awesome. I'm on the Haas VF-TR Series 5 axis Trunnion Mill post.

Haas VF-TR Series 5 axis Trunnion Mill post = misc settings:

"0" it will decide which way to go

"1" will always stay positive (front side)

"2" will always stay negative (back side)