Well I thought I would take a shot at this example.
So, using OneCNC Expert, I modeled the part. It took about 10 minutes. I didn’t rush plus I needed to look up the countersink diameter for the SHCS and tried to find some information on jack screws but came up empty. I’m not a machinist so I am not as familiar with some items as others are.
Then I programmed the toolpaths. This took about 15 minutes, maybe 20 at most. I am sure this is considered slow, but hey I am still learning. Maybe I can learn something here by others critiquing my methods, since my methods come from reading books and posts on forums and no practical experience. Here are my toolpaths:
1. Facing 1 – Top of stock programmed at Z0. Took off 0.015 in Z with one facing pass. Used a 2” face mill.
2. Facing 2 – Bottom of stock. Programmed bottom of stock (top of parallels at Z0), with one facing pass at Z1.97.
3. Facing 3 – Side of stock programmed at Z0. Took off 0.07 in Z with one facing pass. Used a 2” face mill.
4. Facing 4 – Opposite side of stock. Programmed bottom of stock (top of parallels at Z0), with one facing pass at Z3.86.
5. Facing 5 & 6 – Ends were programmed with a profile toolpath. Assumed that the stock is held in a 4” vise. Programmed with a 1” end mill, 0.1” depth of cut.
6. 3/8” SHCS – Programmed with a center drill, drilled thru and counterbored with a 0.5” end mill (helix style toolpath) for the countersink.
7. 3/16” holes – EDM – drilled thru.
8. 3/8”
JS – Programmed with a center drill, drilled thru and counterbored with a 5/16” end mill (helix style toolpath) for the countersink.
9. Text – engraved with a Cut Chain – Constant Z toolpath using 0.015” tipped bit, 0.05” down.
The model was utilized to create boundarys for the facing toolpaths and paths for the profiling toolpath, by extracting those edges. The hole wizard found all the holes in the model, so I didn’t need to extract any edges to create those toolpaths.
As I finished typing this I realized I forgot the chamfer on all edges. So in another 15 minutes (only because I kept changing my mind and then realized some of my lead-ins/lead-outs were on the wrong side of the holes) I generated a chamfer toolpath for the top face for the edges and the holes. Then the bottom face plus the holes. Each was created with part set at Z0. Then the two ends had a chamfer toolpath on the two remaining edges on both ends. Part set at Z0 and the same toolpath ran twice for both ends.
I didn't program the chamfering of the holes from the back side, but from what I have read I guess this can be done with a dovetail tool and I am sure there is a toolpath in OneCNC that can be used for this, just haven't tried it.
Regards,
Chris