[justgary]

All -

I think I have finally broken the 4th axis code, but still have a few questions. I'll get to those later.

I have attached a zip file including two IGES files and a SprutCAM file. The first IGES file, SprutCAM_4th_Axis.igs, is the part for which you want to create a toolpath. The second file, 4th_Axis_Fixture.igs, crudely approximates the 4th axis rotary table, chuck, and whatever else you might want to avoid cutting. Both of them are already included in the SprutCAM file, SprutCAM_4th_Axis.stc. I wanted to make sure you could recreate my work if you wanted to try.

I'm using SprutCAM 2007 build 5.48, so your mileage may vary. Also, note that you will need the recent "MULTIGOTO" post in order to post a G-Code program using this method.

Here are the steps I took (as I recall) to create the toolpath. Please don't shoot me if I forgot a step. You can always pay Dave to help you if you get lost...

1. On the 3D Model tab, Import the part file.
2. Select all of the surfaces of the part (Ctrl-A will do it).
3. Right Click on any of the selected parts. You will see a popup menu.
4. Select 3D Model | Properties, and a popup window titled "Objects Properties" will appear.
5. Select the Machining tab.
6. Uncheck the Double Sided checkbox and then click OK.
7. Select all of the surfaces again if they are not selected.
8. Right Click again on any of the selected parts.
9. This time, select 3D Model | Inverse from the popup menu.
10. Now click on the Machining tab.
11. Select the Machine line and click on the Parameters button.
12. On the popup that appears, click on the Machines tab.
13. Select 4-axis milling machine (A) and click OK.
14. On the end of the menu bar of the program, click on the icon for create coordinate system. It should be the little white rectangle next to the box that says, "Global Mill CS." A popup window will appear entitled, "Definition of new coordinate system (CS)."
15. Click on the Rotary Axis tab.
16. Click in the Position box and type 360. Click OK.
17. Define the workpiece. I simply used a cylinder around the part, along the X axis.
18. Select Machining and click on the New button.
19. Select Tool-End 5D Machining from the Finishing tab. Click OK.
20. Click on the Parameters button.
21. Select the tool. SprutCAM seems to have a bug in that it will only use the center point of the tool to compute Z height in this mode, so you should probably plan on using a Ball Mill. Enter your favorite feed and speed.
22. On the Strategy tab, select Axis Z Position as the Safe Axis, and set the level to something larger than the largest radius of the part. In the case of the example, I used 1.1 inches.
23. At the bottom of the Strategy tab, play with the top and bottom levels until the toolpath is what you want. In this case, I used 0.5 and 0 inches.
24. Also on the Strategy tab, in the Machine State box, select Workpiece Coordinate System and pull down RotAxis 360;0 (the local coordinate system you made in steps 14 through 16).
25. Change Local Coordinate System to RotAxis 360;0 in a similar fashion.
26. Click OK on the Parameters window.
27. Under the Machining tree, click the little plus marks until you see Job Assignment. Select Job Assignment.
28. Add the faces you would like to machine using the Add Drive Faces button.
29. SprutCAM makes a group of the faces you chose. In the box below the Add Drive Faces button, select the group (Group 4 in this example). Click on the Properties button that is on the same line as the Add Drive Faces button. An Item Properties popup will appear.
30. Select the Alternate front side checkbox.
31. Change the step method to Distance (or whatever you want). Change the Step amount to 0.05 (or whatever you want; it defaults to one step).
32. Click OK.
33. Now click the Run button and let SprutCAM create the toolpath.
34. Simulate and enjoy.

The questions: As I mentioned in Step 21, I think SprutCAM has a bug in this mode in that it will only work correctly if you choose a ball mill. Every other tool I tried will crash on the cone shaped portion. I found this before when I tried to get a 4th axis toolpath, and here it is again. You can change to using the side of the mill by choosing Flank on the Strategy tab, which may give a better finish. That may be a way to get a flat but sloped surface (but no sharp corners).

Also, this part is pretty simple. Have any of you tried anything more exotic, like an eccentric cone? Dave's example of a camshaft is eccentric, but also simple in that it only has flat (horizontal) areas to mill. I suspect SprutCAM will fall on its face with a more difficult part.

Try this out and let me know how it goes. Maybe we can resolve the questions by just tinkering with the parameters.

Regards,

- Just Gary

P.S. Well, I tried to attach a zip file. It is way under the max size allowed, but failed to upload several times. Any ideas?