Tool change height is lower than part on mini mill

[Gordon Dawson]

I have a tall part I'm machining, but the Tool change height is lower than the top of part zero. After a tool change I want the Z axis to move up 4.0 inches before the part moves under the tool. I know there is a way to raise "Z" before xy moves, but I don't know how to do that.

Any help would be nice.

Thanks, Gordon

[Chris Rizzo]

Easy and prob safest is use a reference point to send the table to for a tool change. That way you are sure to get the part to the right side of the machine, and not under the tool changer. You can clip tall parts with tools rotating in the carousel just as easily.

[K2csq7]

Gordon, Just use the point toolpath to move the tool to the right point in Z, before your real toolpath starts.

[Mr. Wizzard]

G91 G28 Z0.

That's what i've had to do a few times on some short run jobs.

[Gordon Dawson]

Ok, I added a point move and it worked on the beginning of the drill cycle, but when I was finished drilling, the drill started back down to into the hole so it would of crashed at the end of the cycle. I'll try a point move after the drill cycle and see if that completes it.

[gcode]

Activiate the refence point feature and set an approach and retract point

in the drill toolpath.. that should do it.. though you may have to manually move the apporach Z value

in the posted code

 

 

[Mark V.]

I create a point away and above the part and use toolpaths point and select the point. Do it as the first operation and last.

[Müřlıń®]

G91 G28 Z0.

That's what i've had to do a few times on some short run jobs.

I think I have that line hardcoded into my post.

[Gordon Dawson]

Added the point at the end of the cycle and it worked great.

 

Thanks for the help.

Gordon

[K2csq7]

G91 G28 Z0.

 

On some machines this is not the highest Z will go...

[within a thou]

You could also add A secondary Z point using a seperate co-ordinate system and add it to your code. "G90 G54.1 G0 Z0. P#" and add that before all the first and last moves

[kunfuzed]

On some machines this is not the highest Z will go...

 

Correct. You need "G0 G53 Z4.". G53 is a "one shot" machine coordinates code. No need for switching from G90 to G91 and back.

 

We have this same problem on our Haas GR510 Router. We just moded the safe line in our post.

 

%

O1001;

T1 M6;

G0 G90 G17 G40 G80 G53 Z4.;<------------ HERE

G0 G54 X0 Y0 S5000 M3;

G43 Z.1 M8

 

I'd say that's the easiest fix.

[mkd]

haas control has a tool change at home position setting, but will not raise spindle to the "g53 z4" position automatically. would still need methods shown above.

[kunfuzed]

haas control has a tool change at home position setting

 

Just curious, what does that setting do?

[mkd]

kunfuzed,

it moves the machine to home position before executing every tool change. sorry if it wasn't clear. handy for tool clearance if you have a tall trunnion on the machine.

i forgot the setting number.

i'll need to remember it... my VF-3 is delivered 6/13!!!!

[kunfuzed]

it moves the machine to home position before executing every tool change

 

That's bitchen! I'll have to tell the guys at work about that! They had the post configured to use a misc integer to switch on a "Safe Toolchange" position using G58. Lol