define a high feed cutter

[megaman]

how can a person create a custom tool to mimic that of a modern high feed cutter . when doing high speed surface core mill a facemill will not go down steep angles?

 

im using an iscar high feed with the 8mm inserts if that helps

 

thanks

any info would be appreciated

[gcode]

I just define it as a bull endmill with a .12 corner radius.

[Guest MTB Technical Services]

I do as GCode suggests.

 

You need to be careful in defining the corner radius and pay particular attention to the insert geometry itself.

Ingersoll, for example, has high-feed inserts where the bottom geometry of the insert is a fairly large radius

that actually blends to your typical 1/32, 1/16 corner, etc and then the shoulder has another rather large radius.

The insert itself isn't really rectangular so what the vendor may call out for a radius may not actually be the corner radius you need for the bull-nose definition.

 

If you actually want to create a custom tool, get the TDM tool drawing from ISCAR.

You should be able to actually download the DXF file from their site.

Here's just an example.

http://www.iscar.com/Ecat/familyhdr.asp?fnum=2794&app=&mapp=ML&GFSTYP=M〈=EN&type=1

http://www.iscar.com...3105259〈=EN

 

You can then edit the drawing to only include the right-half of the tool profile and put it in the proper orientation.

Then you can create your custom tool.

[Guest]

I have always drawn it as a custom tool

[Hardmill]

I have always drawn it as a custom tool

 

Same here

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Matthew Hajicek - Singularity]

Remember that the tool profile for verification and the tool definition don't have to match. I define the corner radius as specified by the cutter manufacturer as the "program for" radius, and the toolpaths drive off of this, but then I use a custom tool profile that more accurately represents the tool for verification and stock model.

 

[JoshC]

If you are using X7 and If Iscar can provide you with a DXF (typicaly they are made avalable on the MFG website) of the tool and as long as they set up the DXF properly meeting the ISO 13399 standard (which it should be) then you can simply load the DXF into the new tool manager built into X7 and the tool will come in custom without any need to construct or edit the dxf file. I would typically save the DXF to the same location you keep your tooldb files. Hope this helps

[megaman]

i am trying to make use of all the info here but putting it all together and getting mc to use and show the tool definition does not seem to work. just reverts back to a flat endmill or gives me an hourglass shape.

[JoshC]

i am trying to make use of all the info here but putting it all together and getting mc to use and show the tool definition does not seem to work. just reverts back to a flat endmill or gives me an hourglass shape.

Please send a link to the exact tool you are using off the tool manufacturers website and I will see if i can do a vid.

[megaman]

Please send a link to the exact tool you are using off the tool manufacturers website and I will see if i can do a vid.

 

http://www.iscar.com/eCatalog/item.aspx?cat=3105246&fnum=2592&mapp=ML&app=75

 

 

this is the cutter.

 

i tried to edit the dfx file in mastercam , again i couldnt figure out how to edit the file and make it usable.

 

what steps do i need to do to make this usable for verify and be able to see the tool and get an accurate output of what the part would look like?

 

thanks again

[BBprecise]

I've always done like JParis (Hey John) says make a custom tool. Iscar has the majority of their tools ready for download as a DXF file. If they don't you can request it (done this a couple dozen times) and you should have it with a couple days. My process is as follows, download the file and delete everything not needed to make a wire frame of the tools and make orientate it so the very bottom is at Y0 and the center of the tool is at X0. Create a vertical CL with the short then long dashed line and trim the highest Y axis line (this will be where you want the bottom of your ema, you shouldn't have any other horiz. lines in your file except for maybe at the bottom of the tool at Y0) then scale it so your largest cutting dia when analyzed says it's at "X1.". I always make the wire frame green and put it all on the same level. I've got several different sizes and styles of Iscars feedmills as custom tools. Quite often just using their suggestion of using a bull endmill with a radius works well, but if you have an angled surface in the bottom of a pocket you might need a custom tool. If you don't you could be leaving more material than you want.

[Guest]

I've always done like JParis (Hey John) says make a custom tool. Iscar has the majority of their tools ready for download as a DXF file. If they don't you can request it (done this a couple dozen times) and you should have it with a couple days. My process is as follows, download the file and delete everything not needed to make a wire frame of the tools and make orientate it so the very bottom is at Y0 and the center of the tool is at X0. Create a vertical CL with the short then long dashed line and trim the highest Y axis line (this will be where you want the bottom of your ema, you shouldn't have any other horiz. lines in your file except for maybe at the bottom of the tool at Y0) then scale it so your largest cutting dia when analyzed says it's at "X1.". I always make the wire frame green and put it all on the same level. I've got several different sizes and styles of Iscars feedmills as custom tools. Quite often just using their suggestion of using a bull endmill with a radius works well, but if you have an angled surface in the bottom of a pocket you might need a custom tool. If you don't you could be leaving more material than you want.

 

As Mike says, that is the thing right there. Sure a Bull definition will work but when dealing with the angle into the radius on the bottom, I always wanted to make sure leftover stock condition was as I expected

 

:waving: Hi Mike