Direction not supprted - Samsung mill-turn
It looks like the toolpath "Internal Axial Slot (4)" requires a B-axis to reach that position. Is the head on the machine able to tilt around the Y-axis (the brochure/specification from the link does not mention a B-axis)?
If the machine does have a B-axis, you can modify the Samsung Mill-Turn post to support it by modifying the following:
var gotBAxis = true
There will be further modifications required to match the post up with the machine, but it would be best to check whether the machine has a B-axis first.
Hope this helps,
Tom
Tom Hemans
Technical Consultant
I was getting some strange results so I attempted to sort it out. I moved origin to model face in setup, that is now Z0 in G code.
As for internal trace tool path, if tool orientation is not used, tool crashes into part while entering and retracting.
If I use tool orientation, tool clears and looks on target in simulation but when posted all X coordinates are negative.
I am not sure what is going on here, seems to be conflict of tool actual orientation in Z axis but forced to approach cut from X axis and post has some issue with sorting that out.
I think if you post it as is then remove negative sign from all X coordinates in trace tool path, it will work as intended.
Origin moved to model face, that will be Z0 when you post and all Z depths are in reference to that plane, if you set origin at stock face, your reference point is gone with first cut.
You can still make a part but measuring anything in depth while machining part would require accounting for stock and that's not how we work.
In picture below, each axis is set to point in sink with how they are arranged in machine and view is set to front.
Views and axis orientation in Manufacture and Design are independent of each other so they don't have to be the same.
I personally make them the same because if I want to add a sketch in the middle of programming job I can switch between work spaces and have things in same orientation and in same place.
Often I see sketches out of line with model and in that state it is difficult to gain control of events as they build up to more complexity.
As a rule of thumb you also want to face , rough turn, drill, rough bore, finish turn, finish bore, groove, thread, do mill work and cut off.
Order of operations makes a difference, if you finish turn then drill hole, you may not have same size finished diameter after drilling,... it depends on material.
On subject of tool orientation, rotary tools are oriented so that blue arrow point in direction tool is coming from.
I had an issue with Bush model using tool coming from Z+ direction but requiring orientation in X - direction in order
to make a cut using side of the tool, that I would simply program manually but was trying to get Fusion to do the right thing and I think post is out of sink with concept.
Each axis is pointing to its corresponding orientation in machine, you set part in machine to have G54 work offset .05 below stock face, as set in Fusion setup.