Tool Life Management Setup - Know Your DN, Episode 12 

100% correct.

Thanks for the request! We take all of these request into consideration when selecting content for future videos.

Mike, you are correct. At the time of the video the parameters were all being set to 99 but somewhere recently they started sending them as 999. I will check with the production company and see what we can do about that.

Norah, we have not done a video on tool load management because our partner Titans of CNC has done a great video on how to use it here: ru-vid.com/video/%D0%B2%D0%B8%D0%B4%D0%B5%D0%BE-ZbepcxJAiOs.html

Correct. So that line of code would look something like: G43H99D99Z5.0 - Great Question!

To my knowledge, the only way to turn off the tool life management for a particular tool while using something like Dry Run would be to go in and delete that tool from the tool group.(11:00 mark of the video) There is no way to "suspend" tool life management temporarily. One other suggestion I would have is run the program in Dry Run as many times as needed and then go into the Tool Life page and adjust the amount manually so if I had a tool count of (2) and I dry ran the program 5 times those tools would show (7) uses. I would just highlight that tool and move it back to (2) and then run my program.

Yes it does. If you look in this video at the 9:06 mark, I actually go over how to do this with G10. Great question!

The is option in custom screen - offset - patern for details pls refer operation manual

Rich, you will need to contact your local dealer for service related help as it relates to TSC.

You would simply set up your tools just like I showed on the mill either with the iHMI Tool Management page or using the G10. The only difference is you are calling the group number. So let's say that tools 5 and 10 were sister tools. You designate them as Group 1. Your tool call for using tool 5 or 10 would look like this: T0199. 01= Group 1 99 = the default tool offset that tool groups use. I recommend making your group number the same as the tool number you are wanting to use. So if I was using Tool 5 and it's sister tool was 10, I would designate that group as Tool GROUP 5. That way when I called T0599 it was using tool group 5. If I called T0505 then it was only using tool 5 and offset 5.

Working on a lathe with tool life management is more tricky I think, and this is what he wanted to point out. For example if I want in Group 5 to have the T0515 (not T0505) how should I call it in tool life management mode? Of course we are talking about a twin spindle lathe, this is the tricky part.

@@johnn.katsaoras4958 So each path has it's own tool groups. So as for TT, you would just treat each path as it's own lathe and set up the tool life accordingly. As for calling same tool number but with different tool offsets, you simply would put them in separate groups. So for example, Tool 5 with offset 5 (T0505) would be put in group 1. Then tool 5 with offset 15 (T0515) would be put in Tool group 2. So, when you call it in your program, you would call T0299 for tool group two and T0199 for tool group 1. So in summary, if you have tool numbers with different offsets, just assign that number and offset to a separate group. Hope this makes sense.

The tool life management system monitors either accumulated cutting time or tool usage count for cutting tools which have been registered to a tool life management group. On a standard turning center, up to 32 tool groups can be managed. • Tool life can be preset selectively, either by units of time (# of minutes) or by units of tool usage count (# of times each tool within a tool group can be used). • Cutting time for a tool is recorded by the system when command blocks containing the Gcodes G1, G2 or G3 are executed with a feed rate command (either in G98 or in G99‐ mode). Tool count is recorded each time when a tool group is called. • Tool life for a single tool which has been registered within a tool group can be managed. • Tool life for a number of tools which have been registered within the same tool group can be managed. In such a case, all of the tools within this group must have identical geometric shapes, size and physical properties. Upon tool life expiration of one tool within a group, the next available tool from this group will be selected automatically. • An alarm message referring to expired tool life notifies the user when the tool life on a tool group has expired. Machining can be resumed upon manually resetting the tool life. Programming Notes • Tool life data, tool and tool offset data can be input to the NC by use of a tool registration program as shown on page 3, or by inputting the data, manually. • After inputting the above data, non‐managed tools must be distinguished from managed tools by the tool command as follows: a) To call non‐managed tools, standard tool commands, such as: T0101, T0202, T0303, etc are used. b) Managed tools that have been assigned to a tool group must be called from the NCprogram by use of a tool group command, such as: T0199, T0299, T0399, etc. The first pair of digits addresses the tool group number. The second pair of digits is always 99. It starts tool life management. The system automatically selects the first available, nonexpired tool from within the commanded tool group. Tool offset activation is done, automatically. • Upon completion of machining, tool life management for an active tool group must be cancelled by a command such as: T0188, T0288, T0388, etc. The first pair of digits addresses the tool group number. The second pair of digits is always 88. On machines equipped with an ATC the above cancellation commands must not be used. The M06‐ command cancels tool life management, instead. (See programming notes for MX‐style machines on page 3) Page 2 • When the tool life for all registered tools within a tool group has expired the machining cycle stops at the end of the NC‐program, automatically. An alarm message referring to the expired tool life will occur. Before machining can be resumed the tool life data must be reset manually by the machine operator. Resetting the tool life is done on the tool life management display (see page 4). • Tool life management is interactive with the DOOSAN Tool Load Monitoring System. Tool overload or tool breakage detection signals received from the tool load monitoring system will automatically result in tool life expiration for the active tool which was subject to tool life management at the time when the “tool skip”‐signal was received. Tool Life Management Parameter settings for machines equipped with a turret 1. Set parameter 6800 bit #0 and bit #1 as desired, depending on application. (Please refer to parameter manual B‐63950EN/03). For example: Suppose that on a turning center equipped with a 24‐position turret, tool life management for at least 24 tool groups is required. In this case, parameter 6800, bit #0 and bit #1 should both be set = 1. On a control equipped with up to 99 tool offsets, this setting allows for a maximum of 32 tool groups with up to 4 tools, each group. The maximum number of tool groups in parameter 6813 must be set = 32. Note: After changing above parameter settings, a tool registration program (similar to the one as shown on page 3) should be executed in order to correctly display all of the tool groups in the tool life management display pages. 2. Set parameter 6800 bit #2 either =0 for tool life input by tool use count, or =1 for tool life input by minutes. Settings can be modified for each tool group individually by using the edit feature on the tool life management display pages. 3. Recommended setting for 6800 bit #3=1. 4. Please review the remaining bits on parameter #6800 and set as desired. 5. Set parameter 6800 bit #7=0 6. Recommended setting for 6801 bit#3=1 7. Set parameter 6801 bit #7=0 8. Recommended setting for 6802 bit #0=1 9. Set parameter 6811=54. This sets the tool life restart M‐code. M54 is the parts count Mcode. The purpose for using this M‐code is to update too life data at the end of the NCprogram. Alarms related to tool expiration will occur after execution of this M‐code. Hence, M54 should be inserted near the end of the NC‐program, just before M99 or M30 10. Please review the remaining parameters from 6801 through 6845 and set as desired. Tool Life Management Parameter settings for ATC on MX‐type machines 1. Recommended parameter setting: 6800 bit #0=1 and bit #1=1. The control is normally equipped with 400 tool offsets. By the above parameter setting, either 80 tool groups with up to 4 tools each group, or 40 tool groups with up to 8 tools each group are available. Recommended setting for parameter 6813 = 40, (40 tool groups, 8 tools each). Page 3 2. Set parameter 6800 bit #2 as desired. 3. Recommended setting for 6800 bit #3=1. 4. Recommended setting for 6800 bit #3=1. 5. Set parameter 6800 bit #7=1. 6. Recommended setting for 6801 bit#3=1 7. Set parameter 6801 bit #7=1. 8. Recommended setting for 6802 bit #0=1 9. Set parameter 6811=54. 10. Please review the remaining parameters from 6801 through 6845 and set as desired. Tool Life Registration Program Example: 4‐digit Tool Command 5‐digit Tool Command Explanation O6789 O6789 NC program # G10L3 G10L3 Tool life data input command (Modal command) P1L15 P1L15 P1 = Sets tool group 1 L15 = Sets the tool life units (minutes or tool use count) T0707 T07007 Tool #7, offset #7. Tool assigned to tool group 1 T0808 T08008 Tool #8, offset #8. Additional tool assigned to tool group 1 P2L13 P2L13 P2 = tool group 2 L13 = tool life units (minutes or tool use count) T1424 T14024 Tool #14, offset #24. Tool assigned to tool group 2 G11 G11 End data input command M30 M30 End of program Tool Command Examples for machines equipped with turret 4‐digit Tool Command 5‐digit Tool Command Explanation T0101 T01001 This is an ordinary tool and tool offset command for a non managed tool. Tool life management is not performed. T0 T0 This is an ordinary tool offset cancellation command. T0299 T02999 This is a tool group activation command. It selects a tool from tool group 2. Based on the tool registration example as shown above, tool 14 offset 24 will be selected, automatically. Caution: When executing this command the turret must be located at a safe position to allow tool indexing. T0288 T02888 This is a tool group cancellation command. Tool life management for tool group 2 is terminated. This command must be used after machining with a registered tool group has been completed. No turret indexing or tool offset cancellation will be executed. A tool offset cancellation command can be executed separately after this command, if required.

My h99 is just calling up offset length for t99, on a 5 axis dvf500 with 120 tool pockets. Ant help??