The drilling in fusion looks fine. I would almost 100% guarantee you have something wrong with where you have told the machine zero is vs. fusion.
Some things to check:
- Make sure you are using the same offsets in the program and machine. IE. G54 code and G54 in machine
- Check to make sure where Z zero is set is fusion is the same place you are touching off with probe.
If you can elaborate on the machine you are using that would help. Typically when you are probing, the probe is of a known length and the machine is then measuring all the tools relative to the probe length.
There are really two schools of thought when it comes to setting up a machine for making a part.
The simple way to do this, without a probe just to see if that is the issue somehow is to go with the tool touch off method. Take your edge finder, get x and y for g54. leave G54 Z as 0. Then touch all the tools off the actual part. So the gauge length of the tools is all relative to the Z of that specific part. Downside is you have to touch off tools for every job. Upside is it is very simple, and is often used ALOT in shops doing one off pieces where tools are constantly changing.
The other method... Is best explained in the link below as method 3. Fundamentally what you are doing is setting the length of the tools all off the gauge line of the spindle. Usually the face. So every tool length should be positive... I think. Yeah that should be right. Then you go and when you get a new part and you just have to tell the machine where the part is relative to the gauge line of the spindle and all the tool offsets stay constant. Instead you place a Z offset in the G54. With this method you don't have to retouch tools once they are touched. You can just do one touch-off on the part with the spindle face and you are set.
Where the probe comes in, is that goes in the spindle, and has some gauge length off the spindle gauge line. Same as all your other tools. You then touch off the part and that gives you a G54 XYZ. So possibly in your case that length offset for your probe could be wrong and causing the issue. Or your tool offset for the drill could be wrong as well. Or the part offset in Z for the G54 is wrong. It has to be one of those 3. Cause I really don't see anything wrong with your program.
The other thing you can do for tool touch offs if you never want to touch off tools is what I do. I have a fixture plate in my machine that I fixture everything off off. I touch all my tools off the top of that plate and then never touch them again. When I program my cad, Z zero in the cad is always the top of that plate and I place the part in space where I want it. I never touch off tools or part heights. Just load and go. This is rather advanced and requires good discipline and good habits, but it works very well for repetitive jobs and I didn't need a 6k probe package lol.
Some links to help:
https://blog.caminstructor.com/caminstructor-tips-tool-length-offsets-explained
