Mazatrol Nexus - Line Machining and Tool File - Help me make sense of it

Hi. I'm trying to mill out a fairly simple shape but programming this in Mazatrol is anything but simple. The manual was no help either, it only confused me even further.
The machine I'm using has no Y-axis so I must use the C and X-axis to create a virtual Y-axis.

1. I get this error 434 - "No assigned tool in tool file". Does this mean I can't just define the tool in tool data? I've honestly never used the tool file before because I can't figure out how it's supposed to work.
2. If I do use the tool file, where do the offsets go?
3. How does it know which tool slot to go in?
4. How does it know what direction the tool is mounted in? From the program or what?
5. Where is the radius compensation? All I see is length compensation and the tool file has no compensation whatsoever.
6. In the LINE LFT unit (I assume this is the right unit for this) what exactly do all the parameters mean and which ones are necessary to input?
7. How do I adjust the Z coordinate for the chamfer tool? Surly I must tell it somehow where the top and bottom chamfers start, right?

I got it to do some kind of shape now but it's definitely not right. It's gouging the corners for some reason. I tried adding an extra line move for lead-in but then I get error 693: "Number of Shapes too Large". What does that even mean?

Yes as stated above. The tool file is just providing extra info to the machine for milling tool. It requires you to fill it out basically so it can idiot proof you. Like if you were to tell it to cut 12mm deep per pass but the tool file says the max DOC is 6mm it will fault rather than bury your cutter. It also uses the material to do auto set feed and speeds.

So it does appear as though you filled it out correctly for your endmill and you will need to make one for your chamfer cutter as well. It needs to know the angle of the tool and how big the tip is(meaning what diameter the flat nose of the tool is). It needs that stuff because it will use it to calculate where the tool needs to cut to do your desired chamfer size or fault if you go too big. It will automatically use closer to the nose or the outside if there is an obstruction near either. (typically defined as Interference Z and R) (those aren't shown here but should be if you were using a chamfer left) On the line left the interference in the top of the unit is referring to radial interference and it is determining your Axial interference based on the depth you are cutting. The chamfer tool will cut the top edge of your milled feature.

Then you create the Tool Data for those tools and that is where it gets the comp from. It will use the cutter diameter to offset for the unit you are using. Line left is climb milling so that is likely what you want.

Read the bottom right of the screen as you are learning Mazatrol. It's called conversational for a reason. It is having a conversation with you. Any time you are over something there will be a question in the bottom.

I'm a mill guy so I can't really help you with the shape without a machine in front of me. I could fumble trough it if I saw what it was asking but can't off the top of my head.

The other guy is right though. The blue color of your first two lines indicates them as a start point so it's seeing that as 2 shapes. Delete and re write the second one. This likely happened because you inserted a line at the top when it had already made the first a start line.

I tried to break this stuff up so it would be easier to reference but hopefully I was able to help.

csteen said:

The number of shapes to many is because when you added a line to your shape sequence, you added it as a start to a new shape.

Click to expand...

I see. So the machine needs to know that the first line is the first line. That makes sense.

csteen said:

Not sure why you have two chamfer tools in your tool sequence, should only need one.

Click to expand...

I was thinking I could do both the front and back chamfer in just one unit but I had to copy the unit and "lie" a little to do the back.

csteen said:

The tool file is for defining the tool itself which looks like you have done correctly, I cannot see your tool though. The Tool Data page is where you tell the machine where the tool is located and the direction it is pointed in the machine.

Click to expand...

Aha. So I have to define it in both Tool Data AND Tool File. Seems kinda redundant, but whatever.

csteen said:

I suggest you try and forget all previous CNC programming experience while reading the Mazatrol manual and look at it with an open mind, all the information really is there.

Click to expand...

You know, I guess it's my bad, but I expect systems like this to follow some kind of logic and reason. It's like they said, hey, this process is too simple. Let's complicate it by adding a bunch of useless parameters for no reason. It's just aggravating.

Nagol said:

On the line left the interference in the top of the unit is referring to radial interference and it is determining your Axial interference based on the depth you are cutting.

Click to expand...

I'm not sure I follow. I tried changing it but I didn't notice any difference in the tool path. Would have made sense to just use a stepover value as cam software does. I couldn't figure out how to add extra roughing passes so I had to copy the unit and add more FIN-R to control the stepover.

Nagol said:

Read the bottom right of the screen as you are learning Mazatrol. It's called conversational for a reason. It is having a conversation with you. Any time you are over something there will be a question in the bottom.

Click to expand...

Well, not really. First of all, it's all written in Engrish, almost impossible to understand sometimes. Second of all, it doesn't really explain what each parameter is supposed to be. Like APRCH-1 and APRCH-2, for instance. It just says "approach point 1" and "approach point 2". That to me makes it sound like it's two different points they're referring to. But how can you define a point with just one value? Doesn't really make sense. What they should have said is "approach point X" and "approach point Y".

That being said, it would have been nicer if it could just handle this automatically based on stock size, previous operations, and what have you. Now I had to use an excessively large approach point to not clip the corners of the part. Makes it cut a lot of air for no reason. Not good.

On you generation control the tool will only take multiple passes axially not radially. The chamfer tool will only cut once. It just determines what part of the tool to use based on parameters. As far as approach points I'm thinking this might have been your issue with it chopping the corners off. You basically always will use the auto set for those and when you run the program or the tool path it will come up with a safe approach coordinate.
It also likely says approach 1 and 2 since the axis are dependant on unit type and axis being used. Generally for your machine I think it would be X and C
Set approach to auto and see what you get.