We have recently moved to NX9 from NX7.5 and we have this tool problem.
In NX7.5 when we are changing the tool holder and the (OS) Offset value but the tool data remains, and if we create a new operation with the same modified tool it will just retrieve the tool data from the library like the speed and pitch or depth of cut value. But now in NX9 we don`t know if we are just missing some default setting to automatically retrieve tool data from library even when we change the (OS) Offset or holder, so that we don`t have to input again the tool data in each operation with the same tool.
Solved! Go to Solution.
I am not sure exactly what the issue is.
If you change the Tool Insertion Offset of the tool, and then Set Machining Data, the parameters are recalculated based on the new tool length sticking out of the holder.
If this is about always updating the operations, then as Joachim said, be sure the customer default is set.
Yes I have checked the set automatically in operation, but if I change just the tool holder it prompt a warning (You have modified a tool which was retrieved from an external library. Do you want to keep your modification?) so I will select yes option, and when I create another new operation with the same tool that I have changed the holder i will prompt a warning (No entry was found in the Machining Data Library that matches the current Part Material, Tool Material, and Cut Method.). In NX7.5 even if I change the tool hoder, this warning don`t popup, as long as I don`t do anything inside the tool tab parameters.
Are you calculating the machining data based on part material, tool material, and cut method?
Or are you using the tool machining data tied to the library tool libref?
Changing the offset should mark the tool as having been modified, but it will still know it's original libref.
This looks correct to me - once you change the tool, it is no longer a library tool.
Let me explain...
A library tool is an assembly, including the holder. If you edit it, it is no longer a library tool. Changing the offset has the same effect as changing the diameter - the system knows that the tool in your work part is not the same dimensions as the one in the library.
Tool machining data is for library tools only. When you set machining data, since the tool is no longer a library tool, the system does not look at the tool machining data table, I goes directly to calculating the feeds and speeds, and does not find the necesary inputs.
You did not see this in the old release because the tool was not getting flagged as editied when the offset changed - a problem that we fixed.
If you want to keep and reuse the tool with the new offset, I suggest you export it to the library, either replacing the previous tool, or creating a new one. If you create a new one, add tool machining data for the new libref.
A tool from the library is not editable, this is the purpose of a library tool.
Library tools are meant to be always the same and to not change at all.
If you like to change the tool at will and keep the machining data for the diameter and the tool length, then you need to switch from "tool machining data", which is bound to a fixed library reference, to "machining data", which is bound to diameter and length of the tool.
In general it is total nonsense to change a tool retrieved from a library, since that is representing a tool that you can get from the tool preparation department by just showing them the tool ID (library reference).
Usually changing library tools is even locked, so you can't do that at all.
Production: NX10.0.3, VERICUT 8.1, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0
Employees of the customers, together we are strong
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide