misc integer to send tool home, m00, then come to operator, m00?

[jgary]

Hello,

 

First of all i am using X2, and programming for an Okuma HMC with a Fanuc 18i controller.

 

I have been reading up on these mi's. I am just having trouble figuring out where to put this information in the post.

 

Here is what i want to do:

 

After i rough a bore, I want to send the tool home and program stop so the operator can check size. Then I want to bring the tool to the operator with a custom M135, and program stop to dial boring head, and/or rotate/change insert.

 

Thanks in advance for your time and effort.

[crazy^millman]

Well not to sound like a broken record, but your dealer is a great resource.

 

Now I would look to MPMASTER since it already has this built in it, except for the coming to the operator. Add that and you are home free.

 

You can also do a search for this has been explained many many times with lots of examples.

[jgary]

I have looked at many posts on here talking about manual entry, misc values, canned text, and I think the way to go is with some misc values, I am just trying to figure out if pcanceldc$ would be a good place to put this sort of thing...

 

 

This forum is a great resource to have, I just wish I could contribute 1/2 as much as I have gained.

 

Thanks to all who participate on here.

Great Job!!!

 

[ 12-07-2007, 12:10 PM: Message edited by: jgary ]

[Guest]

CREATE 2 SAME TOOLS WITH THE SAME NUMBER. USE THEM FOR ROUGHING AND FINICHING OPERATIONS. WHEN YOU POST THE 2 OPERATIONS, THE MASTERCAM ASK YOU THAT THERE IS 2 OPERATIONS USING THE SAME TOOL NUMBERS; YOU NEED TO POST TOOL CHANGE; JUST SAY YES. AND HERE YOU GO.

[Guest]

quote:

---

After i rough a bore, I want to send the tool home and program stop so the operator can check size. Then I want to bring the tool to the operator with a custom M135, and program stop to dial boring head, and/or rotate/change insert.

---

You could do this using a force tool change, you would need no adjustment to the post, just create the path twice and on the second use the force tool change option. then using canned text, you could get the M135 code to output. That to me would be the easiest way to accomplish this.

 

I've used canned text to do something similar in the past, here's some eaxamples

 

code:

---

if cantext$ = one, [pbld, n$, sm00, e$

pbld, n$ "(CLEAN CHIPS)", e$

]

 

if cantext$ = two, [

pbld, n$, sg00, "Z6.0", sm09, e$

pbld, n$, sg91, "G28", "Y0.", e$

pbld, n$, sm00, e$

pbld, n$, "(CHANGE CLAMPS)", e$

pbld, n$, sg00, *g_wcs, sg90, pfxout, pfyout,

*speed, sm03, e$

pbld, n$, sm08, e$

]

if cantext$ = three, [

pbld, n$, "M201", e$

]

 

if cantext$ = four, [

pbld, n$, "M200", e$

]

 

if cantext$ = five, [pbld, n$, sm00, e$

pbld, n$, "(ROTATE TO DEGREE)", e$

]

 

if cantext$ = 6, [pbld, n$, sg91, "G28", "Y0.", e$

pbld, n$, sg90, *g_wcs, "X0.", e$

pbld, n$, sm00, e$

pbld, n$, "(LOOSEN AND RETIGHT VISE)", e$

pbld, n$, "( DO NOT OVERTIGHTEN)", e$

]

 

if cantext$ = 7, [pbld, n$, sg91, "G28", "Y0.", e$

pbld, n$, sg90, *g_wcs, "X0.", e$

pbld, n$, sm00, e$

pbld, n$, "(CHANGE SCREW LOCATIONS)", e$

]

---

I have also added an option into an MPMaster post for a home move on top of the mi10 option they built in

 

code:

---

if (mi10$=four & (op_id$ <> last_op_id | (op_id$ = last_op_id & xform_op_id$ <> op_id$))) | (tlplnno$ <> prvtp & ret_on_indx), pstop

---

pstop has a call to to phome postblock

 

code:

---

phome

pbld, n$, "G91", "G28", "Y0.", e$

pbld, n$, *sm00, e$

---

There really are a few ways to accomplish what you need.

 

Home some of the examples offer some direction

 

[ 12-09-2007, 09:41 AM: Message edited by: JParis@CNC Programming Solutions® ]

[Bryan Johnson]

using the misc page is the way to go for this.

 

there is a good example of this on the FTP site. I think the file name is Haas_VF.zip.

It is setup to use mi1.

[Trevor Bailey]

use the force tool change just like what john said. you will need to find that section of the post and just add the line for a table move: pbld, n$, "G0", "G90", "G54(or whatever)", "X0", "Y0", e$

 

it only takes minutes to do.

 

for the mpmaster post that inhouse puts out, i add this to it specifically for checking op's between same tools and i will add the table move when toggling on the M00 feature also.

[jgary]

hey guys,

 

thanks for the replies... sorry it has taken so long for my reply. I am trying some of these things out today. I think the 'force toolchange' is a great idea.

 

John,

 

I have a couple of questions about your comments.

 

quote:

---

if cantext$ = one,.....

---

First of all, where is all of that cantext code located in your post?

 

quote:

---

code:

---

 if (mi10$=four & (op_id$ <> last_op_id | (op_id$ = last_op_id & xform_op_id$ <> op_id$))) | (tlplnno$ <> prvtp & ret_on_indx), pstop 

---

---

Secondly, on the mi10 line with the pstop and phome, basically, does that make the program have a stop and return home on every toolchange when mi10 is set to four in your example?

 

Thanks for all of your help.

[Guest]

jgary,

 

Send me an email as you don't have an available one in your profile

[jgary]

John,

 

You have mail.

 

Jeramiah

[jgary]

I have to take off for a couple hours. I'll be back later today though...

 

once again,

 

thanks

[Post dept]

jgary,

 

Yes, use the misc int 10 to force the M00 then you'll get all your startup stuff as well.

 

There's an mpmaster_okuma post available that does this (then you can just add your custom stuff to the mi10$ logic). Just have your dealer request the post on your behalf.

 

Brett

[jgary]

Good day to all,

 

Thanks for all of your help I have got it the way I want it now. I can not say how helpful this place has been. You guys rock!!