Tool library . Fanuc Robodrill w/ 31i b5

[Jacob79]

Hi guys

I'm new to the fanuc controller, but have 15-20 years of experience with Siemens and Heidenhain.
My workplace bought a brand new Robodrill with 21 tool holders.
On both Heidenhain and Siemens you can have e.g. T50 in holder nr.1. and you just call T50, but on the Fanuc I can only have T1 in holder nr.1 etc.
Is there any way to get about this, because we have a rather comprehensive tool library already setup in MasterCam and we are used to identify our tools by their respective number?

On Heidenhain/Siemens you save the length etc. with the tool number.
On Fanuc you save it under a H-number.
Do you save the tools used, along with a tool offset list with every program, like a project? If so, how is this done?

Regards Jacob
 

[Guest]

What version of Mastercam?

 

Moved to the Industrial forum as this is a Mastercam question, not so much a machine one

Edited May 24, 2017 by Guest

[Jacob79]

11 minutes ago, JParis said:

What version of Mastercam?

 

Moved to the Industrial forum as this is a Mastercam question, not so much a machine one

Mastercam 2017

[Codeworx]

On Fanuc the machine can only see tool numbers equal to the carousel. Robodrill 1-21, or 1-14 on eco model.

You could use any number over 21 as the offset number(your existing tool library) but the Tool call number/position in machine will have to be 1-21.

IE:

T1M6 (Machine pocket 1)

G43 H50 (length offset "tool" 50)

G42 D50 (Dim offset "tool" 50)

[Colin Gilchrist]

Program your job as "normal", selecting your existing Tool from your Libraries. You can either:

1. Set the option in the Machine Group Properties > Tools Tab, to "Assign Tool Numbers Sequentially",
2. Or, program as normal, then Select All Operations > Right Click > Renumber Tools

The defaults for having Tool # = Pot # on the machine, can often be "customized" by the Machine Tool Builder, but it will cost you some money. Typically the "M06" tool change G-code calls an internal Macro Program, and that program can be customized. The same goes for the Tool Registers.

According to my Fanuc 31i "B", manual (B-64484EN), the tool code can be up to 8 digits.

Quote

NOTE

1. The maximum number of digits of a T code can be specified by parameter No. 3032 as '1' to '8'.
2. When parameter No. 5028 is set to '0', the number of digits used to specify the offset number in a T code depends on the number of tool offsets.
   1. When the number of tool offsets is 1 to 9:           Lower-order one digit
   2. When the number of tool offsets is 10 to 99:       Lower-order two digits
   3. When the number of tool offsets is 100 to 999:   Lower-order three digits

 

 

 

[Jacob79]

7 hours ago, Codeworx said:

On Fanuc the machine can only see tool numbers equal to the carousel. Robodrill 1-21, or 1-14 on eco model.

You could use any number over 21 as the offset number(your existing tool library) but the Tool call number/position in machine will have to be 1-21.

IE:

T1M6 (Machine pocket 1)

G43 H50 (length offset "tool" 50)

G42 D50 (Dim offset "tool" 50)

Thank you for your reply.

Yes that is properly the way i am going to do it. The problem here as I see it, is that you have to manually edit the program to put in the D and H numbers for each tool. I cannot see there is any possible way of making a post capable of doing that for you = Chance of human error....

[Jacob79]

4 hours ago, Colin Gilchrist said:

Program your job as "normal", selecting your existing Tool from your Libraries. You can either:

1. Set the option in the Machine Group Properties > Tools Tab, to "Assign Tool Numbers Sequentially",
2. Or, program as normal, then Select All Operations > Right Click > Renumber Tools

The defaults for having Tool # = Pot # on the machine, can often be "customized" by the Machine Tool Builder, but it will cost you some money. Typically the "M06" tool change G-code calls an internal Macro Program, and that program can be customized. The same goes for the Tool Registers.

According to my Fanuc 31i "B", manual (B-64484EN), the tool code can be up to 8 digits.

 

 

 

Hi Colin thank you for your reply

I am aware of those 2 options in Mastercam and i am currently using the 1. example that you gave.

I am actually thinking of asking Fanuc to customize the M06 if possible and the Tool registers.

 

I am not sure that i undertsand your example of this solution:

The maximum number of digits of a T code can be specified by parameter No. 3032 as '1' to '8'.

When parameter No. 5028 is set to '0', the number of digits used to specify the offset number in a T code depends on the number of tool offsets.

When the number of tool offsets is 1 to 9:           Lower-order one digit

When the number of tool offsets is 10 to 99:       Lower-order two digits

When the number of tool offsets is 100 to 999:   Lower-order three digits

 

Is it possible for you to make a small example?

In my manual i can only see that you can make 3 digit tool numbers only if you asign them to tool groups when using the tool life management function.

 

 

 

 

[Newbeeee™]

6 hours ago, Colin Gilchrist said:

Typically the "M06" tool change G-code calls an internal Macro Program, and that program can be customized.

Hmmmmmm...... I don't think so Tim (am I showing my age?  )

Well, on our old Robos with a 31iA5 control, the toolchange macro was compiled and couldn't be changed. Ohhh, and we tried...

And we then wrote our own, changed the parameters to call the new 9001 toolchange program etc, and it ignored it. The machines only wanted to use its inbuilt and hidden (to us at least) macro.

And just for the record, I had the UK Robodrill 'guru' trying to do this for us, so it wasn't Newbeeee at the controls

 

[Colin Gilchrist]

4 hours ago, Jacob79 said:

Hi Colin thank you for your reply

I am aware of those 2 options in Mastercam and i am currently using the 1. example that you gave.

I am actually thinking of asking Fanuc to customize the M06 if possible and the Tool registers.

 

I am not sure that i undertsand your example of this solution:

The maximum number of digits of a T code can be specified by parameter No. 3032 as '1' to '8'.

When parameter No. 5028 is set to '0', the number of digits used to specify the offset number in a T code depends on the number of tool offsets.

When the number of tool offsets is 1 to 9:           Lower-order one digit

When the number of tool offsets is 10 to 99:       Lower-order two digits

When the number of tool offsets is 100 to 999:   Lower-order three digits

 

Is it possible for you to make a small example?

In my manual i can only see that you can make 3 digit tool numbers only if you asign them to tool groups when using the tool life management function.

 

 

 

 

I was just pointing out some of the Parameters on the Fanuc 31i B control, that allow you to tweak the "T" code settings. I can't give you an example of changing the settings, because this is always dependent on the Machine Tool Builder. As Newbeee mentioned, you'll need to get Robodrill to make the modifications, and they may just say "No", depending on how they've built the PLC ladder and configured the HMI.

[jeff]

4 hours ago, Jacob79 said:

Thank you for your reply.

Yes that is properly the way i am going to do it. The problem here as I see it, is that you have to manually edit the program to put in the D and H numbers for each tool. I cannot see there is any possible way of making a post capable of doing that for you = Chance of human error....

You don't have to do that. I never do. Check your settings.

[Jacob79]

22 hours ago, Colin Gilchrist said:

I was just pointing out some of the Parameters on the Fanuc 31i B control, that allow you to tweak the "T" code settings. I can't give you an example of changing the settings, because this is always dependent on the Machine Tool Builder. As Newbeee mentioned, you'll need to get Robodrill to make the modifications, and they may just say "No", depending on how they've built the PLC ladder and configured the HMI.

Ok thank you 

[Jacob79]

22 hours ago, jeff said:

You don't have to do that. I never do. Check your settings.

That sounds exactly what i'm looking for, but maybe i have been staring  myself blind in Mastercam settings, because i can't seem to figure this one out.

Is there any possible way you can tell me how to do that please?

 

[taperlength]

On 5/24/2017 at 10:33 AM, Jacob79 said:

I'm new to the fanuc controller, but have 15-20 years of experience with Siemens and Heidenhain.
My workplace bought a brand new Robodrill with 21 tool holders.
On both Heidenhain and Siemens you can have e.g. T50 in holder nr.1. and you just call T50, but on the Fanuc I can only have T1 in holder nr.1 etc.
Is there any way to get about this, because we have a rather comprehensive tool library already setup in MasterCam and we are used to identify our tools by their respective number?
 

I had a similar situation recently and copied the existing library, renumbered the tools and then made a cheat sheet showing showing the new tool numbers next to the old numbers.  Changing the tool numbers on the Robodrill if even possible, would be confusing to the operator because the numbers are on the magazine right above the spindle.  The machine uses a 30 taper spindle so its not going to be sharing the actual tools with other machines any way.