Bore drill starts above material, and doesn't go through bottom, contrary to simulation

[alex.ciepluch]

I have a 0.125" thick aluminum panel that I am trying to drill several 0.05" diameter holes in with a 3/64" square endmill via bore drilling operation. I even made the endmill drill 0.05" past the whole depth to ensure a clean exit hole.

Here is a screenshot of the simulated tool path in Fusion. You can see the bore drill operation clearly goes through the material.

Here are my geometry parameters for the tool path:

Now, I am exporting the g-code with "Easel / f360-easel-revision" post to my inventables x-carve router. The g-code looks correct as in the starting z=0.125 and each hole goes down to z=-0.05 when I look in notepad.

In the native router software Easel I am importing the g-code as my toothpath, and at this point I can zoom into the tool path and see the helix drilling operation is starting above the material top (shown below).

Indeed when I follow the Easel setup to define my material and zero the z-axis, my toolpath only goes about halfway through my 0.125" material.

I'm wondering what I'm doing wrong that my tool path is not finishing through my material? I'm pretty confident in my Fusion CAM setup, so wondering if its maybe an issue with Easel software.

[seth.madore]

Can you share your NC code and your Fusion file here?

[alex.ciepluch]

@seth.madore  I've attached the .nc and .f3d files

[DarthBane55]

If the code is good, most likely work offset is set wrong or tool height.  When it goes to the start height, stop it there, measure how far up above the material your tool is, and it will most likely be 0.15+0.0625 above.

*EDIT: I've seen your code now, so stop it at Z0.275.  You set your Z offset below the material, so at Z0.275, your tool should be 0.150" above the stock.  Check that.

[alex.ciepluch]

I tried what you suggested by eliminating the remainder of the g-code after the Z0.275 command on line 11. My endmill stopped above the material, and I measured the distance from material to endmill (i.e. from model top to endmill).

This measured approximately 0.275" per the g-code. So I'm not sure what new information I've gained. 

[DarthBane55 · Accepted solution]

No, if it measures 0.275" above your material, you've gain the information that I was correct... 😁

Your Z zero origin is set under the material (in fusion).  In the code, the tool goes to Z-0.05, and that is 0.05" below the material, as you had explained.

Now, the top of your material is then 0.125", because your material is 0.125" thick (in fusion).

0.275" is from your Z origin, which is under the part.  0.275-0.125 = 0.150".  When you go Z0.275, the distance from the tip of the tool to the top of the material should measure 0.150".

If you say it measures 0.275", it means that in the machine, you have set your Z origin to be on the top of your material, but in Fusion, you have set it on the bottom of it.  These 2 need to match.  

Either change Fusion to have the Z origin on top of the material, and recode, or change your origin in the machine to be under the material, like you did in Fusion.

Actual life: Z zero on top of material, code goes to Z-0.05", your actual holes are only 0.05" deep.

[Spencer.AC]

If you are measuring .275 distance from the top of the material to the bottom of the tool prior to engaging the feed, it is your work offset. The tool should be stopping .150 above the material not .275. You can either change your Setup work coordinates to the top of the part or comp your Work Offset -.125 in the controller.

[alex.ciepluch]

Thanks for the quick feedback. The issue was that in Fusion my model origin was the bottom of my panel, but when I zero the z-axis in the machine setup I use the top of the panel.