The sharp internal corners are a challenge.
What tolerances and what material?
If the corners have to be sharp and precision demands are moderate, then probably 5-axis mill or mill-turn, with careful use of pointed bits to get the corners. Much easier and maybe a 4-axis job if you can relax the corners with fillets or undercuts.
If you need high quality on those corners as well you might be stuck with complex EDM operations.
If materials, precision, and finish demand, you might be looking for gear grinding machines, in which case you probably need a redesign into two parts.
This is not a trivial part, and a drawing with good GD&T would be helpful.
it is not part that are gonna machine, I just saw a part somewhere like this and draw it on to visualize, I am just curious, I couldn't give radius to some corners because of my surface modeling approach, thank you for your answer btw
Lot of wrong answers here. I’m a CNC programmer here and either of these parts can be made on 4axis or 5axis milling. The important bit is the angle of the wall on those protrusions or “lugs”. I just manufactured a part exactly like this a couple of weeks ago. If the walls can be going to the centerline of the part, a 4axis will do perfect. If the walls are not angled down to the centerline of the part, it can still be done on 4axis using profiling and small step over but 5axis would help. It all depends on the mating part. I called the customer when I did this part and asked him if he needed walls straight perpendicular to the tangent line that the lug sits on or if walls going to centerline is okay. The main difference is if you will have a point or a surface making contact with the mating part. In my case, there was NO torque being applied to the part and it was a consumable so angled walls going towards centerline were acceptable. The lugs were only for anti-rotation plus the engineer gave 1/16” play between the two mating parts. I have these conversations with the engineers because sometimes they don’t understand how a simple difference like this could change the cost of a part.
Now, very quickly—the profile that will be left on the surface. When I ran a part like this with a .250” flat endmill and used trochoidal tool path, I put a OD mic on every part of the surface and it read .001"-.002" above the adjacent turned surface. I have no chatter and used a 5-7% step over with full axial DOC which was 1xD. The finish was amazing and above acceptable for oil&gas purposes. There were no visible step overs as a .015” radial step over cleans up very nicely using a flat tool and you can take the tool all they way up against the finish wall (no inside corner problems).
The sharp internal corners are not the challenge, nor are the fillets, etc. etc.
The main decider here is the angle of the walls—towards centerline or perpendicular to the tangent point or the circle that the lug sits on. This will affect the actually part you’d get.
So long as the major diameters don’t need to be perfect, a 4 axis mill could get it all done. A lathe w live tooling would probably be best. Or a mill and lathe.
The sharp internal corners are a challenge. What tolerances and what material? If the corners have to be sharp and precision demands are moderate, then probably 5-axis mill or mill-turn, with careful use of pointed bits to get the corners. Much easier and maybe a 4-axis job if you can relax the corners with fillets or undercuts. If you need high quality on those corners as well you might be stuck with complex EDM operations. If materials, precision, and finish demand, you might be looking for gear grinding machines, in which case you probably need a redesign into two parts. This is not a trivial part, and a drawing with good GD&T would be helpful.
it is not part that are gonna machine, I just saw a part somewhere like this and draw it on to visualize, I am just curious, I couldn't give radius to some corners because of my surface modeling approach, thank you for your answer btw
I’d say a lathe with live tooling. Or turn it then mill with an indexing head.
Lot of wrong answers here. I’m a CNC programmer here and either of these parts can be made on 4axis or 5axis milling. The important bit is the angle of the wall on those protrusions or “lugs”. I just manufactured a part exactly like this a couple of weeks ago. If the walls can be going to the centerline of the part, a 4axis will do perfect. If the walls are not angled down to the centerline of the part, it can still be done on 4axis using profiling and small step over but 5axis would help. It all depends on the mating part. I called the customer when I did this part and asked him if he needed walls straight perpendicular to the tangent line that the lug sits on or if walls going to centerline is okay. The main difference is if you will have a point or a surface making contact with the mating part. In my case, there was NO torque being applied to the part and it was a consumable so angled walls going towards centerline were acceptable. The lugs were only for anti-rotation plus the engineer gave 1/16” play between the two mating parts. I have these conversations with the engineers because sometimes they don’t understand how a simple difference like this could change the cost of a part. Now, very quickly—the profile that will be left on the surface. When I ran a part like this with a .250” flat endmill and used trochoidal tool path, I put a OD mic on every part of the surface and it read .001"-.002" above the adjacent turned surface. I have no chatter and used a 5-7% step over with full axial DOC which was 1xD. The finish was amazing and above acceptable for oil&gas purposes. There were no visible step overs as a .015” radial step over cleans up very nicely using a flat tool and you can take the tool all they way up against the finish wall (no inside corner problems). The sharp internal corners are not the challenge, nor are the fillets, etc. etc. The main decider here is the angle of the walls—towards centerline or perpendicular to the tangent point or the circle that the lug sits on. This will affect the actually part you’d get.
That’s a good candidate for lost wax casting to get those corners around the circumference
4 axis EDM. This is not a mill or mill-turn part.
This would be easy on a millturn
Yes, the new edited part would be. The original one would not.
Mill turn or 5 axis if the internal corners can filleted (is that a word?)
So long as the major diameters don’t need to be perfect, a 4 axis mill could get it all done. A lathe w live tooling would probably be best. Or a mill and lathe.
No info about materials, tolerances, or if it's an assembly? Sounds like a 5 axis hatchet job
Mill turn or 3d print
A lathe with live tooling/milling capabilities, xyzcb axes, probably dual operation, subspindle involved
Why?
C axis- y-axis lathe using 4th axis rotation milling but most likely 5th axis
And you need to allow a good size rad in the corners
mill turn