Can you force a tool change?

[Go Navy]

I know this is an easy one but, what I would like to do is have mastercam force a tool change at the begining of each operation even if the next operation uses the same tool. The reason I would like to do this is so that I can start machining a part at almost any point as long it is at the begining of a tool change. We run a lot of very long parts and must secure our machines at night no matter where it is in the program.

 

thanks in advance for all the help

Al

[Jimmy Wakeford from Barefoot CNC]

Depending ont the post you are using you can test the variable op_id against prv_op_id in the ptlchg0 postblock. If they are not equal call ptlchg else run through ptlchg0.

This will let you tool change on different ops, but wont change during the same op.

 

Jimmy

[Mark H]

In the operation manager open up the toolpath. Then on the first tab select Change NCI there should be a check box with force tool change select that for each toolpath you need the toolchange.

[chris m]

You may need to block skip the toolchange depending on your control as many don't like seeing tool numbers called that are already in the spindle

 

C

 

What kind of machine? If it is an Okuma there are better ways

[Go Navy]

Thanks to everyone!! Mark H solution was just what the Dr. ordered. I don't know what we would do without this forum.

 

Have a great day everyone

Thanks again

Al

[Rekd™]

Al, if this is something you want to do EVERY toolpath, you can set it in the defaults.

 

NcUtils

Def Ops

Defaults

 

Click the SAVE button

 

Now open each operation you use, and make that change. Then save it all and every time you create a new operation, those values are in place.

 

'Rekd

 

[ 09-03-2003, 06:59 PM: Message edited by: Rekd ]

[Trevor Bailey]

I am curious. If you add the toolchange to every operation, will the tool retract to machine home(Z) at every operation?

[crazy^millman]

Depends on the machine Mazak's wouldnt unless the parameter was set to. Fadal will not sure about Haas's been so long since i ran one or other machines. I would put the block skip in there also so I could by bass them till I needed it.

 

Just a little food for thought on running your machine over night we run our 16 to 20 hours sometimes. At 75 dollars an hour is that machine runs 20 hours without soemone being here just made $1500 dollar profit toward my deparment for the month. The machine is not going to do anything you dont tell it to. We also have 4 machine so in the rare days I can get that out of them we make $6000 for that time profit. Just my 2 cents worth.

 

Crazy Millman

[CR@seyer]

I have that problem, how do I change the post so that I can get the g28 home move and shut off coolant / spindle etc. and not get the tool change? I need this for the times when I am using a single tool to machine a part, (i.e. plastic / sheet metal profiles etc.) and I need to send the machine home and turn it all off so that the operator can change clamps and the like safely.

 

Thanks

Clayton

[crazy^millman]

I think you would want to d othat with your canned text just add it at the end of an operation or the begining. Define one of the Canned texts at your G28 Z0 and go from there. You can also so it for everytime but think you might like the canned text. If you want to do it then just have to add that into your nulltool change part of the program to get it to do it at every operation and toolchange. Look at the Mpmaster psor at emastercam I have modified it an like what it does

 

Crazy Millman

[Rekd™]

My HAAS posts will return after the end of each program, (M30), to the machine zero on Y and Z.

 

No tool change if the first tool = last tool. It's a pretty simple edit for your post. If interested, lemme know.

 

'Rekd

[Trevor Bailey]

At the M30 in my post, I add a fixture offset that is dedicated just for the table to move forward. Pretty easy change as Rekd said.

 

 

pbld, n, "G0", "G90", "E OR G?", "X...", "Y...", e

pbld, n, first_tool, e

"M30"

 

[ 09-03-2003, 10:08 PM: Message edited by: Trevor Bailey, from Barefoot CNC ]

[crazy^millman]

Oh I Misunderstood your posting mine would only do you good if you wanted to do it between operations Trevor and Rekd have put you on the right path Young Luke. May the Mastercam force be with you.

 

 

 

Crazy Millman

 

[ 09-03-2003, 10:21 PM: Message edited by: Millman^crazy ]

[Rekd™]

quote:

---

pbld, n, "G0", "G90", "E OR G?", "X...", "Y...", e

pbld, n, first_tool, e

"M30"

 

---

Actually, you might want something like..

code:

---

if t <> first_tool, pbld, n, first_tool, e

"M30"

---

..that would test to see if the first tool is the same as the current tool, if true, do nothing, if false, change tools.

 

'Rekd

 

[ 09-03-2003, 11:35 PM: Message edited by: Rekd ]

[Trevor Bailey]

pbld, n, *first_tool, "M06", e

pbld, n, "M30", e

 

This is what I put in all my post. Never failed me yet. Rekd, you make everything too "scientific" looking.

[Rekd™]

LOL, Trevor. You're prolly right, all that work to save 5 bytes of data.

 

'Rekd teh Anal Retentive

 

[ 09-04-2003, 08:44 AM: Message edited by: Rekd ]