Heidenhain TNC 355 / 155 / 151 selecting tools extra to the carousel

I have a CNC mill (Beaver Partsmaster) with a TNC355 and a 16 tool carousel.

On occasions it would be very useful to to able to manually load a tool for a one off but for the life of me cannot find how to do it !

At the moment I just have to re-define a tool by removing one and inserting the substitute and go thought the tool length offset process each time.

Ideally I'd like to have these (not very often used) tools already pre-measured in a rack awaiting manual loading at the appropriate part of the program.

Is this possible ?

I'm sure the process must be the same for the TNC151 / 155 / 355 as they are all very simiar

DO you have to enter an M6 when you call a tool? Depends on how the PLC is written I think

If so you could manually change a tool and call the new tool without an M6

The newer controls have a tool table and a pocket table, so you can theoretically call a tool [say tool 17] that is in pocket 5

IF you do not need to use the toolchanger then use TOOL DEF to define the tool[thus saving its radius and length in the program] and TOOL CALL like I do on my old knee mill. I guess I would see how your machine reacts to a tool call that is out of range[IE tool 17]

To call a tool it's just Tool Call T# Z Speed cr/lf

If I call a tool in MDI it is Tool Call (button) T# Z Speed then Manual Stop M6 but if the tool number is out of range of the tool table (16 tools) then it objects that there is no tool def.

If I try to make a sub program with tool defs in, although I can enter the tool number I can't enter the length or radius values so I presume the fact that there is a tool table prevents the question being asked.

I haven't tried setting the tool table length to more than the tool changer has pockets as I don't want to tangle things up !

Huh, I can redefine a tool on the fly, It is how I do a rough finish pass. Incremental length and radius
In programming mode it does not allow you to enter a TOOL DEF?

I start a new program - say #100 - in EDIT mode,tell it the mode ie metric in my case, input a TOOL DEF, it opens a box to enter the tool number, but according to the manual when that's been entered boxes should appear for tool length and radius, but they don't

The small program now contains a Tool Def but it only has the tool number but of course not the other parameters !

Check paramters, there might be one that disables it tho I cannot think of why

if MP225 is set to something other than 0, then it forces you to use tool library (0 program) and you cannot set tool length and radius via the "TOOL DEF" command in the edit mode, at least that is how it works with the software version of the 355 on my machine (Mikron WF41)

my machine had a tool changer, had to remove it, so I set the MP225 to zero and have to fully define each tool before using it in a program, modified CAM post accordingly, that was the workaround to not get the PLC errors when tool call is performed and TNC finds out that some parts on the machine aren't there any more

That's very helpful, thank you.

I'm now wondering if it is possible to make the tool table longer than the carousel, maybe 24 tools in the table and actually 16 in the carousel - will it perhaps demand a manual tool change for tool numbers over 16? Or will it totally muck up the tool changer - not sure I want to risk that by experimenting !

what command on your control actually starts the tool change?
If you have to use L M06 to initiate the tool change, then you might not brake anything if you increase the MP225 above the number of actual tool pockets, but you have to be very mindful of this in your programs and always return the original tool changer pocket tool back into the spindle to continue using ATC, here is what I mean:

(total number of tool pockets 17, MP225 set to 50)

...regular program with TC...
tool def 1
tool call 1 S5000
l m06
(cutting program)
stop m05
(here you do the manual tool change to the tool 50)
tool def 50
tool call 50 S200
l m03
(cutting program)
stop m05
(manual tool change back to the tool 1)
tool def 1
tool call 1 S5000
(now you can either continue with tool 1 or change to another tool in the tool changer)

everything depends on how the ATC program is written, if you have some logic programming experience and electrical diagrams, you might be able to figure out how it works and whether increasing MP225 above the number of physical pockets breaks anything, but those PLC programs aren't exactly easy to read if you don't know what all the markers are used for

I've never actually managed to work out how to view the PLC program on the TNC355.

(I did manage to crack the Siemens 820T control that I have on a Beaver TC20S lathe, teach myself 'Step 5' the code it's written in,identify about 75% of the flags and make some significant changes but that took 6 months of late nights and gallons of coffee and a spinning head!

have a look at this thread I started a while ago - tnc 355 plc

the code to access the PLC is there, so is the description of how it may be split in 2 parts, first 2048 commands and then additional 1024, Mikron has fully geared spindle, meaning it has to change gears to change speeds, and that takes quite a bit of that PLC memory, so if you have a more conventional spindle, then you might not need to look into the 2048+ portion

andrewmawson said:

I haven't tried setting the tool table length to more than the tool changer has pockets as I don't want to tangle things up !

Click to expand...

^^that's how I would do it. On a 530 you can append lines in the tool table. Not sure of the 355. Fully define that tool. Since it doesn't have a pocket, with a proper PLC, it should go to a manual tool change position and unlock the door. At least a Mikron will.