post question

[Rick46]

Im wanting to modify my post where when it does a tool cahnge that it will move the table all the way to opposite side of machine away from the tool changer arm.. Normally it changes tools right where previos operation finshes its last cut..this can cause crashes when I change to a tool that sticks out of the holder to far.. so I am thinking why not modify my post to move the table out of the way to avoid this from happening.. Is this possible to do in my post and if so how and where..lol.. thanks..

[Guest]

Before digging in to change the post have you tried using a reference point to change its tool change position?

[Rick46]

nope not sure how..but open for any suggestion..

[Chris Parish]

Hey:

 

Under the misc. integers... I have G28 X0., G28 Y0, or G28 X0.Y0.

 

pretract

etc etc

 

pbld, n$, sgabsinc, *sg28ref, "Z0.", e$

g28_rtrn = prv_mi7$ #Set flag for safe toolchange position

pbld, n$, *sg28_rtrn, e$

 

Then make a string select like this...

 

#Safe Toolchange Position

sg280

sg28X0 "G28 X0." #reference return in "X"

sg28Y0 "G28 Y0." #reference return in "Y"

sg28XY0 "G28 X0. Y0." #reference return in "X" and "Y"

sg28_rtrn #Target string

 

fstrsel sg280 g28_rtrn sg28_rtrn 4 -1

 

 

Hope this helps....

[Rick46]

If I use the G28 X0 line it will take the table and work piece right under the tool change arm .. this is where I do not want my work piece to be during a tool change..is there a different value I can use to make it go to the opposite side of machine away from the tool change arm..and can I modify my tool change area in my post to reflect this every time I do a tool change.. thanks...

[Justin Beebe at Folsom Tool]

sr_7626,

 

We have a similar situation with one of the machines we have. Our machine uses a 9001 program to initiate the tool change whenever there is a M06 in the program. We control where the mchine positions itself before the tool change in the 9001 program. I can't remember off hand exactly what the code looks like but if your machine uses a 9001 program for tool changes I can look at the code tommorrow and post it for you. Let me know if you that will help you.

[nofalloff]

This is a little crude but effective. you could find a place that the table is safe and load that location in to a high work offset number as x0 y0. I have 99 work offsets in the form of G53OXX so this is easy for me. The other advantage to doing it this way is in your post you can just have an output statement that inserts "G0 G(offset#)X0Y0" at the beginning of your tool change

(n$, "blah blah blah", e$).

Don't forget to call back you working offset at the end of your tool change.

I think that's (pbld, n$, pwcs, e$).

Please someone correct me if I'm wrong.

[Rick46]

cncjb.. thanks for your reply.. the machine in question does use a 9001 program for all tool changes.. any help you can throw my way is much appreciated.. thanks

[Dave Ball]

quote:

---

Before digging in to change the post have you tried using a reference point to change its tool change position?

---

As John said this is your simplest option. Fanuc code for this would look like..

code:

---

G0 G91 G30 P2 Z0

G0 G91 G30 P2 X0 Y0

---

This is used just like G0 G91 G28 X0 Y0 Z0 only it lets you set the position to return to. parameter number 1241 contains the value (actual machine axis positions) of each axis for P2. FYI 1242=P3 1243=P4 As I said this is for a Fanuc 16/18 control not sure what your using but most machines have a second, third and fourth reference position but you may have to dig around to find the parameters to set them up for use.

[chris m]

Rick, we have a Mori-Seiki VMC with a rotab on it and the M-code macro [9001] has an X move away from the rotary before the toolchange. The way it is done is a combination of what nofalloff said and what cncjb has. If you want to do this ALL of the time, and if you have a spare WOFS location what I'd do is move the machine where you want it to change tools, call that G5X X0.Y0. and then edit your macro to add a G00 G5X X0.Y.0 before the toolchange starts. To be extra safe you might want to use G10 in your macro to set this WOFS position every time in case some smart guy blows away the WOFS location. In order to edit the 9001 program you'll need to find the parameter that will allow you to edit 'protected' programs.

 

If you only want to do this once in awhile then I would suggest using Reference Points from within Mastercam

 

C

[Justin Beebe at Folsom Tool]

sr_7626@natl

 

The safe tool change position for our machine is:

 

Machine Y0

Machine X-22.0

 

The 9001 program looks like this:

 

O9001(TOOL CHANGE)

M9

G0 G28 G91 Z0. M5

G91 G28 Y0.

G90 G53 X-22.0

G40 G49 G80

M6

G90

M99

 

 

The G53 controls the X-22.0 move. It sends the machine to the machine position of X-22.0 from any X start position. I did not make this 9001 program and this is a little confusiing to me because I thought a G91 was used with a G53 but that will not work I tried it. Keep in mind that on this particular machine X0Y0Z0 never change. If you want to try something similar I suggest doing a tool change with no tool in the spindle to avoid a collison. I hope this helps I am having a very busy day so I had to rush through this post. If you need more help let me know.

[Tinhman]

If you need to move the table away for every job then you should modify your post. But if you just need for a couple special job then i think the best way to do it is use the reference point as John said ( There is a little box on the lower right corner in the tool parameter page).

Hope it help.

Tinhman

[Rick46]

thanks a bunch guys.. I am gonna try the options listed here and see what works best for my situation..

[Rick46]

quote:

---

quote:

--------------------------------------------------------------------------------

Before digging in to change the post have you tried using a reference point to change its tool change position?

 

--------------------------------------------------------------------------------

 

As John said this is your simplest option. Fanuc code for this would look like..

code:

--------------------------------------------------------------------------------

 

G0 G91 G30 P2 Z0G0 G91 G30 P2 X0 Y0

 

--------------------------------------------------------------------------------

 

This is used just like G0 G91 G28 X0 Y0 Z0 only it lets you set the position to return to. parameter number 1241 contains the value (actual machine axis positions) of each axis for P2. FYI 1242=P3 1243=P4 As I said this is for a Fanuc 16/18 control not sure what your using but most machines have a second, third and fourth reference position but you may have to dig around to find the parameters to set them up for use.

---

I am using a Fanuc 18i-M controler.. I see the parameters you mentioned above and they are set at 0 for the time being. Are you saying I can input a relative position in here and have mastercam post the code to call out these parameters and go to the values I input in my control when I run a program . ex.. tool changes..

[Dave Ball]

Yes, its exactly like a toolchange position. In fact your toolchange position should be listed in parameter 1240. However its not a relative position, its a "machine" position. Manually move your machine table to the position you want, then write down the "machine" positions for all axes, make sure you write down the values under the "machine" heading while in the position screen. Enter these values into the appropriate axis column under parameter 1241. Now in your program just use this...

code:

---

G0 G91 G30 P2 Z0

G0 G91 G30 P2 X0 Y0

---

to make the machine go to that position. Just change the P value to 3 or 4 to position to the values in parameter 1242 and 1243 respectivly. The G0 G91 G30 in the second line is redundant and not needed, but it helps operators see what is going on. I use this to position for all sorts of things...bring the vise/setup to the operator by centering in X and out in Y at the end of the program...position mid cycle to check sizes...position prior to B axis rotation...The list is endless.

 

HTH

[john316]

.

 

quote:

---

O9001(TOOL CHANGE)

M9

G0 G28 G91 Z0. M5

G91 G28 Y0.

G90 G53 X-22.0

G40 G49 G80

M6

G90

M99

---

The G53 is an absolute call from the machine zero. A G0G90G53X0Y0 would go to the machine zero position. You can find a safe place for your toolchange and use these in your toolchange macro or hardcode the codes in your post something like this.

 

G91G28Z0

G90G53X-22.Y0.

 

hth.

 

.

[Justin Beebe at Folsom Tool]

john316

 

Thanks for clarifying the G53. I knew it worked in our toolchange macro I just didn't know why it worked.

[mgsanchez]

quote:

---

O9001(TOOL CHANGE)

M9

G0 G28 G91 Z0. M5

G91 G28 Y0.

G90 G53 X-22.0

G40 G49 G80

M6

G90

M99

---

I do something similar for the same reason except that I alias my o9001 program as a M-code (M16 in my case). Since I don't have to do this very often, I just change all M6's to M16's in my machine editor.

 

Or... If you need it every time you post, you can change your post to output your "new" M-code instead of a M6.

 

Mike

 

 

My Program

 

O9001(M16 TOOL CHANGE)

G0 G90 G49 G53 Z0.

G0 G90 G53 X-60.0 Y-20.0 (your XY position may differ)

M6

M99

 

.