Showing results for 
Search instead for 
Do you mean 
Reply

Tool Machining Data by Method

Hello,

 

I need to have a little bit different behaviour for "Set Machining Data".

 

The users need to have one value for roughing and one value for finishing. Because of this, I tend to use two different tool_machining_data.dat files. One for finishing and one for roughing and drilling.

 

Unfortunately, the cut method is not available in the tool_machining_data.tcl code. This is only available in the machining_data.tcl. But machining_data.tcl doesn´t know anything about the libref of the tool.

 

Did any one of you have a similar problem and found a solution?

 

Best regards,

Joachim

Best wishes,
Joachim

In production NX 11.0.1.11 D3
10 REPLIES

Re: Tool Machining Data by Method

Tool machining data is only to be used with tools that have the same feeds&speeds despite of the part material and the cut method.

It is more or less meant for special tools, reamers and taps.

 

If you need feeds&speeds based on cut methods, use the machining data.

 

What is the need to have feeds&speeds related to library reference in this specific case?

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: Tool Machining Data by Method

If I'm understanding what you're doing, we are trying to set up a similar solution here.  We have dedicated tool chains in our machines.  We tap test our assemblies and then run test cuts for slotting, rough profiling, and finishing.  We then need to be able to have 3 speeds and feeds for a tool.  These tools are in the library and we want to tie the speeds and feeds data to the lib ref number in NX.

Jake Hardwick
CNC Programmer
Senior Aerospace AMT
Production NX8.5.3.3 Beta testing NX10.0.1.4

Re: Tool Machining Data by Method

You would have to edit the Tcl code used to apply tool machining data to include some parts of the machining data Tcl code.

This is not easy but doable, never have done this, since we are happy how things work now.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: Tool Machining Data by Method

Hi Stefan,

 

I am fully aware of the current (9.0.3...) NX CAM functionality.

 

We have a in-house tool database in which end user departments have added to each mill tool specific feeds & speeds values for roughing and finishing. In order to be able to translate this to NX CAM, the simplest solution seems to be to be able to distinguish the values to be used with a dedicated method group.

 

Best wishes,
Joachim

In production NX 11.0.1.11 D3

Re: Tool Machining Data by Method

Hi Stefan,

 

what about the interpolation algorithm that is used in machining data? Our NX CAM consultants as well as some key users are having trouble understanding it. I know the NX help section about how interpolation is done. I have also read the TCL source code.

Also, for the integration of the in-house database this would either require a complete reinvention of all feeds&speeds parameters.

I don´t like to again customize a TCL I have to maintain in the future.

 

Best wishes,
Joachim

In production NX 11.0.1.11 D3

Re: Tool Machining Data by Method

The interpolation is done with a tolerance of 10% for the diameter and the tool length.

I have disabled the interpolation by ratio, since that applied values for a 20mm face mill to a 2mm ball mill.

 

We also have introduced different tool materials for end mills and ball mills to better distinguish between the machining parameters.

 

So I would suggest to fine tune by using different materials.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: Tool Machining Data by Method

I dont know much about this, but here is what i did.

 

We created custom methods like HSM_RGH, RGH_Slot, FIN, SURFACE_RGH, SURFACE_SEMI_FIN, SURFACE_FIN ECT.  We then made a few custom OPDO, MATO, and TMCO that all read from a giant cutting data excell sheet imported into the feed and speed library.

 

its a total pain to set up,  but we get the exact feed, speed doc, woc on each and every tool we select.  where it gets tricky in machines with resident tooling.  we have to edit the tool length in the excell file and tool library by .001 and enter the exact data into the LIBRF#.  this forces nx to see an exact match ond only output the proven feed / speeds for this tool when either rgh / fin ect.

 

attached is the excell file to we imported.

Re: Tool Machining Data by Method

Hi Stefan,

 

thanks for your guidance.

 

We will perform the following changes with NX9.0.3-MP2 D1:

 

For users of our internal tool database: Based on the cut method (only roughing and finishing) we will choose the correct feeds and speeds value. In the referenced release, the cut method will be available in the TCL.

 

For users of the native NX tool database: We will use customized tool materials to distinguish between tool vendors and tool types. Additionally, we´ll rewrite the set machining data (machining_data.tcl) algorithm to use a linear interpolation that our users can anticipate. In that interpolation we´ll get rid of the consideration of the tool length and just use the diameter.

 

Thanks to the flexibility with the tcl scripts we are able to do just what we need.

 

Best wishes,

Joachim Schraitle

Best wishes,
Joachim

In production NX 11.0.1.11 D3

Re: Tool Machining Data by Method

Hi dforsythe,

I understand. My colleagues an me think the user should not bother too much with cut methods (except for roughing, semi finishing, finishing). Therefore we'll stick to the tool material trick. This has to be done once, but using it is much simpler. We have the cut methods because of offsets and to distinguish feeds & speeds parameters.

Best regards,
Joachim
Best wishes,
Joachim

In production NX 11.0.1.11 D3

Learn online





Solution Information