Cancel
Showing results for 
Search instead for 
Did you mean: 

2 speeds for the same tool

Pioneer
Pioneer

Hi

i use center dril for chamfer and for cleaning scabies in machining.

i want to automatically get speed 1 for chamfer and speed 2 for scabies at the same tool.

how do i do this?

 

Amnon

15 REPLIES

Re: 2 speeds for the same tool

Siemens Pioneer Siemens Pioneer
Siemens Pioneer

Hello @Amnon!

I believe that you can procede in a lot of ways, but, without know the cnc command and machine type, it's so dificult, but, follow some informations that i belive be valuable

1-You could define your machine to use the rotation based in the diameter of the tool, and then, put 2 tracking points. For each tracking point a different cutting value.

2-Use different operations (1 for drilling and another for chanfer).


WBR
Marco Silva

Siemens PG SU Brazil

Re: 2 speeds for the same tool

Is it a combination center drill with a pilot dia, or a spot drill?

When deburring, is it for holes, or are you using a milling operation?

Mark Rief
Retired Siemens

Re: 2 speeds for the same tool

Siemens Genius Siemens Genius
Siemens Genius

If you are looking to automate the speeds for the same tool in different operation types, say a center drill used in spot drilling and in planar profile for chamfering, then you can edit the Machining Data Libraries. Insert new cut methods named SPOT DRILL and CHAMFER under the Cut Method tab, then go to the Machining Data tab and select the Tool Material, Cut Method (the ones you just created), and the Part Material, then select Insert. You will then enter the Edit Machining Data Record dialog and input the feeds, speeds and other information you want automated for a certain diameter tool. Do this for both new cut methods you created.

 

Once you have created this custom machining data, you will then be able to use it automatically by selecting the Set Machining Data button in the Feeds and Speeds dialog of an operation. However, this only works if you use the machining method, tool type (diameter and tool material) and workpiece material that the machining data was set for.

 

Let us know if this is what you were looking for.

Re: 2 speeds for the same tool

Valued Contributor
Valued Contributor

If you are using a Fanuc control you can add a spindle marker in the start of path events and change the spindle speed as needed per operation. I can't do that on our Heidenhain though. It only allows 1 spindle speed per tool.

Re: 2 speeds for the same tool

Genius
Genius
On Heidenhain you can add a TOOL CALL and S spindle speed command in the middle of the path. Just omit the T#.
Glenn Balon
Production: NX 11.0.1.11 MP7 Primarily CAM

Re: 2 speeds for the same tool

Pioneer
Pioneer

Hi

thank you, but i work with fanuc 18. and i want auto selection of feed and speed according to operation type.

 

Re: 2 speeds for the same tool

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Since this sounds like a process you want to capture.  You could make a template part with the operations, tools and speeds and feeds already defined.  Then just create the operations when needed.

 

John Joyce, Manufacturing Engineer,
Senior Aerospace Connecticut
www.senioraeroct.com
Production: NX11.0.2.7, Vericut 8.0.3
Development: Tcl/Tk

Re: 2 speeds for the same tool

Pioneer
Pioneer

Thank you for solution.

i want to select the right speed and feed only by select operation type.

jkane1 sent me answer that i try and hope will work, i dont understand how to attach the tool to his process.

 

regards,

 

Amnon

Re: 2 speeds for the same tool


Amnon wrote:

Thank you for solution.

i want to select the right speed and feed only by select operation type.

jkane1 sent me answer that i try and hope will work, i dont understand how to attach the tool to his process.

 

regards,

 

Amnon


To use set machining data, the operation needs a tool material, part material, and cut method. Then this combination must be in the database. Once this is set up it works great, but you will need to learn about it to set it up. OOTB you can experiment by using the HSM parameters - there are good combinations for those.  

Tool Machining data is locked to a specific tool, and ignores the other parameters, so I would not use that.

Mark Rief
Retired Siemens

Learn online





Solution Information