KD Fastener custom tooling

[Damon Nabors]

Is anyone using the custom tool that Hafele sells to cut the rafix holes? I purchased one, but I can not get the machine to go and pick it up. I have it set as drill only and the diameter matches the diameter of the hole pattern. Just curious how to set it up.

Thanks,
Damon

[FredHirsch]

Damon,
Is it picking up a different tool and interpolating? You might try moving that tool up to #1 in the tooling group and see if that does the trick. If it is set to drill only it should not use for any other opps.
Fred

[Damon Nabors]

Fred, that's right, it is picking up my 3/8 tool and interpolating the hardware hole. I will try moving it up to number 1 and see what happens.

Thanks, Damon

[Forrest Chapman]

Damon,

In the bottom left corner of settings there is a check box "Run pockets that are 1 arch and 1 line as a drill when the line touches edge of part". You must have this checked.

Make sure your tool is setup .79" in diameter also. You will have to add .06 to your daylight in order to get the full drill depth because of the tip. Don't worry about the tapered flange. If you are useing the lipped cam it will cover it but you will also have the option to use the flush cam.

The tool manf. say to run the tool at 4000 rpm. If you do this your plunge will have to be about 100 ipm. I run the tool at 10000 rpm and plunge at 300 ipm. It works for me but you decide.

If you are setting the tool in a standard 10mil collet remember that it has the chance of working free because the flat spot warps the collet. I've been using an adaptor that my uncle machined for me. Its a 3/4" sleeve with a 10 mm bore and a set screw. Fits right in a 3/4" collet. I use the same ones for 5mm, 8mm, and 10mm drill bits all having 10mm shanks that I use often.

If everything is setup corectly the tool will last for a long time.

Forrest

[Damon Nabors]

Thanks Forrest for the information. I was curious about the flat spot and the collet after I received the tooling. I ordered a 10mm collet for the tool, but I think I am going to do as you did with the sleeve.

Once again, thanks

Damon

[Damon Nabors]

I can't get it to work for some reason. I Set the tool up for .79 Diameter, I went into CN and set the tool up under tooling as Drill only, 10k RPM. 300IPM. Do I need to choose interpolate or anything? I also have the box checked in settings "Run pockets that are 1 arch and 1 line as a drill when the line touches edge of part". It just wants to pick up the 3/8" tool and interp. the hole.

I double check that the hardware hole editor is set at .79" for the hole.

Any other suggestion???

Damon

[Forrest Chapman]

Damon,

I think you need to get on the phone with Ryan H.

Forrest

[Damon Nabors]

Yea, I am going to have to call in Tuesday. It would have been nice to have been able to use the tool this weekend though. I am sure it is something simple.


Thanks,
Damon

[Daniel Vonderheide]

Damon,

Did you move the tool up to operation 1 in the tooling setup? The machine goes through the operations in order looking for a tool it can use and selects the first one it comes across. Because of this, if your 3/8 tool is set as a lower operation number, the machine will use it if it's a viable tool. We suggest setting the operations starting with any odd tools such as this and then your largest drill bit working to your smallest and then your largest router bit working to the smallest. This way, any special tooling is checked first for use and then normal tooling. If you have any questions, call me at 1800-221-3865 ext.245.

[Damon Nabors]

Yee Haw, with your help I got it to work. Moving it up to number 1 did it, but I did notice that it would be nice if there was some way of changing tool priority, rather than having to manually rearrange everything and reset the tool parameters. Just a thought, but thanks to everyone that helped out, we are cutting at full speed again.

Damon