Skip to Content

SiePortal

The integrated platform for your product selection, buying and support workflow - bringing together Industry Mall and Online Support.

SiePortalDeutsch

Search

Home
Support Support
{{(apiData.Support | filter:{'rank':1}:true)[0].title}} Support
- Menu temporary not available
- Menu temporary not available
- Menue temporary not available
- {{item.title}}

Products & Services
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
Support Support
{{(apiData.Support | filter:{'rank':1}:true)[0].title}} Support
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
MySiePortal MySiePortal
{{(apiData.MySiePortal | filter:{'rank':1}:true)[0].title}} MySiePortal
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
Cart ({{apiData.CartCount}})

Navigation

Program to update tool length

Created by: ggorr at: 3/22/2021 5:55 PM (5 Replies)

Rating (0)

Thanks 0

6 Entries

3/22/2021 5:55 PM	Rate (0)
ggorr Posts: 10 Rating: (0)	Hi All I have a 840d control and I'm wondering if there is a way to update tool lengths by running a program that will do this. We have a preset machine for setting our tool lengths and we are able to have the machine create a program for our Fanuc Machines that we run and it updates our tool lengths and rad values. I just wondering if it it possible to do this on Siemens. The reason being we only have a 30 tool carousel and have a number of repeat part just now and are changing tools often so it to try and eliminate error when putting in tool lengths Thanks Graeme
ggorr Posts: 10 Rating: (0)
Suggestion To thank Quote Answer

3/23/2021 1:45 AM	Rate (0)
nulizhang Platinum Expert Joined: 10/17/2007 Last visit: 1/19/2026 Posts: 4579 Rating: (416)	For 840D it is absolutely possible to update toll length during machining. Normally that would be done by the machine builder before design and configuration the machine. For a live update, your machine should have a measuring tool such as Renshaw touch prob and configure with Siemens "measuring cycle" If you "just wondering if it possible to do this on Siemens." --I think my answer is good for you. ggorr Hi All I have a 840d control and I'm wondering if there is a way to update tool lengths by running a program that will do this. We have a preset machine for setting our tool lengths and we are able to have the machine create a program for our Fanuc Machines that we run and it updates our tool lengths and rad values. I just wondering if it it possible to do this on Siemens. The reason being we only have a 30 tool carousel and have a number of repeat part just now and are changing tools often so it to try and eliminate error when putting in tool lengths Thanks Graeme
	If you like my comments please use "Thank" bottom left or Rating Top right
Suggestion To thank Quote Answer

3/23/2021 9:20 AM	Rate (0)
ggorr Posts: 10 Rating: (0)	Hi We have a Zoller tool setter and looking for it to output a short program that can be ran on the machine that will update the tool lengths and rads. So if possible to do this I was just wondering how the layout would be. We don't have a Renishaw touch probe on this machine the tools are issued for our tool store. Thanks
ggorr Posts: 10 Rating: (0)
Suggestion To thank Quote Answer

3/23/2021 4:59 PM	Rate (0)
ggorr Posts: 10 Rating: (0)	Hi All I have got this working using the following, $TC_DP3[1,1]=101.010 ; Length $TC_DP6[1,1]=25.00 ; Radius $TC_DP15[1,1]=-0.02 ; Wear But my problem is now that this is only working with the TNo marked up on the attachment and not the tool No I'm using for tool change. I'm lead to believe this is what is known as the internal tool number and you can see below that it changes once we get to tool 22. Is there a way of changing this number to match the Tool ID or getting the above command to update information above using Tool Id instaed of TNo. Thanks Graeme Attachment InkedIMG_7256_LI.jpg (230 Downloads)
ggorr Posts: 10 Rating: (0)
Suggestion To thank Quote Answer

3/25/2021 10:52 AM	Rate (0)
CNC600 Posts: 455 Rating: (77)	Usually You have to strengthen the ToolSetter to generate a File with the following content, transfer this program to Your control and run it: N10 DEF INT MyNewDuploNumber, MyNewToolNumber N20 DEF STRING[31] MyNewToolName N30 MyNewToolName = "BALL9" N40 MyNewDuploNumber = 1 ; select an instruction to create a tool, pending on Your requirements ;MyNewToolNumber = NEWT ("BALL9", 1) ; Fixed ToolName, fixed DuploNr ;MyNewToolNumber = NEWT ("BALL9") ; Fixed ToolName, automatically generated DuploNr ;MyNewToolNumber = NEWT (MyNewToolName, MyNewDuploNumber) ; ToolName & DuploNr from Block N30/N40 N50 MyNewToolNumber = NEWT (MyNewToolName) ; ToolName from Block N30, automatically generated DuploNr N60 $TC_TP2[MyNewToolNumber]=MyNewToolName ; ToolName N70 $TC_TP3[MyNewToolNumber]=1 ; Size left N80 $TC_TP4[MyNewToolNumber]=1 ; Size right N90 $TC_TP5[MyNewToolNumber]=1 ; Size up N100 $TC_TP6[MyNewToolNumber]=1 ; Size down N110 $TC_TP7[MyNewToolNumber]=1 ; MagPlaceType N120 $TC_TP8[MyNewToolNumber]=2 ; ToolState N130 $TC_TP9[MyNewToolNumber]=0 ; ToolMonitoring N140 $TC_TP10[MyNewToolNumber]=0 ; ReplaceTool N150 $TC_TP11[MyNewToolNumber]=0 ; ToolGrouping N160 $TC_TP_PROTA[MyNewToolNumber]="" ; ProtArea definition N170 $TC_TP_MAX_VELO[MyNewToolNumber]=0 ; maxSpeed N180 $TC_TP_MAX_ACC[MyNewToolNumber]=0 ; max accel N190 $TC_TPC1[MyNewToolNumber]=0 ; OEM specific data ; for CuttingEdgeNumber = 1 N200 $TC_DP1[MyNewToolNumber,1]=110 ; ToolType BallEndMill N210 $TC_DP2[MyNewToolNumber,1]=9 ; CuttingEdgePosition N220 $TC_DP3[MyNewToolNumber,1]=100 ; Length = 100mm N230 $TC_DP6[MyNewToolNumber,1]=4.5 ; Radius = 4.5mm N240 $TC_DPNT[MyNewToolNumber,1]=5 ; NoOfCuttingEdges = 5 N250 $TC_MOP3[MyNewToolNumber,1]=0 ; Prewarning numebr of pieces N260 $TC_MOP4[MyNewToolNumber,1]=0 ; remaining number of pieces N270 $TC_MOP13[MyNewToolNumber,1]=0 ; setpoint of pieces N280 M2 The key is the instruction NEWT for creating a new tool and the instruction DELT to delete an already existing tool (not shown in this sample) The used bunch of ToolValues in the program is pending on the configuration of Your tool management. Additionally some tool values are not changable with these kind of instruction, therefor special instructions exist. Pending on the configuration and the SW-version of Your control additional restrictions become effective (loaded tool in magazine...) Check the programming manual for further information and instructions around NEWT (chapter 6.10) Attachment Function Manual Tool Management Chapter 6.10 NC language commands.pdf (312 Downloads)
CNC600 Posts: 455 Rating: (77)
Suggestion To thank Quote Answer

3/26/2021 9:38 PM	Rate (0)
Steve_A Advanced Member Joined: 4/28/2015 Last visit: 1/16/2026 Posts: 69 Rating: (10)	If the tool you want to modify is the active tool, you can use: $P_AD[n], where n is: Active tool offset; n = 1...31 n=1-25 $TC_DP1 to $TC_DP25 n=26 $TC_DPCE (optional) n=27 $TC_DPH (optional) n=28 $TC_DPV (optional) n=29 $TC_DPV3 (optional) n=30 $TC_DPV4 (optional) n=31 $TC_DPV5 (optional) If you want the tool number of the active tool, use $P_TOOLNO HTH, SteveA

Suggestion To thank Quote Answer

|

Share this page:

Share this page on...

Follow us on