Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

2D Adaptive Clearing Helix Ramp Type Helical Ramp Diameter For Through Holes

david
Enthusiast

2D Adaptive Clearing Helix Ramp Type Helical Ramp Diameter For Through Holes

david
Enthusiast
Enthusiast

I'm cutting 3.2mm and 3.5mm holes in a 2mm thick piece of CFRP with a 1.6mm end mill using 2D Adaptive Clearing and a Helix type ramp. In order for Fusion to create the toolpath for the 3.2mm holes, I must set my Helical Ramp Diameter to 1.5mm and my Minimum Ramp Diameter to 1.5mm -- 1.8mm for the 3.5mm holes --; otherwise, it results in an empty toolpath. What is the relationship of these values to whatever it is I'm cutting? Is there some formula that determines what is an appropriate value for ramp diameters? I just want to know what the values actually mean and how they correlate with my end mill and the hole diameter. Thanks!

0 Likes
Reply
Accepted solutions (1)
1,716 Views
4 Replies
Replies (4)

Trigg3r
Advocate
Advocate
Accepted solution

Nice and simple this one. The hole is 3.2mm diameter, your tool is 1.6mm diameter. If the tool helically ramps into the stock at anything more than 1.5mm diameter then it'll already be over the diameter of the hole you're trying to cut.

 

1.5mm diameter helix on the centreline of a 1.6mm tool gives 3.1mm total circumference meaning it has .05mm stepover left to cut to reach size. Any more on the helix diameter and there would be nothing left to cut. :slightly_smiling_face:

 

As a side note, its good practice to make the ramp diameter to be equal to or slightly less than the tool diameter ( to avoid those awkward moments when ramping with a none center cutting tool :face_with_open_mouth: )

0 Likes

david
Enthusiast
Enthusiast

Thanks. That was an easy one.

0 Likes

Anonymous
Not applicable

Here is what I have observed with my cnc machine

1. machine ramps down in slightly smaller diameter than desired hole.

2. machine expands outward to finish edges of the hole, cutting full depth of the hole.

My machine broke an end mill because it tried to finish the hold at full depth (step 2). Is there any way to avoid this where the entire hole is ramped with a helical fashion? Autodesk insists on finishing the hole at full depth which the endmill cant take.

0 Likes

a.laasW8M6T
Mentor
Mentor

I'm sure the endmill CAN take it if you use the correct cutting parameters, as I do this all the time, in steel, tool steel, stainless and aluminium.

 

It sounds like adaptive isn't really the correct toolpath to be using if the hole is only just larger than the tool.

 

The 2D bore tool path will helix the hole to size, in one continuous helix, if you want to avoid side milling with the full length of the tool.

 

If the tool is close to the size of the hole you should also consider reducing the feedrate so the peripheral feed is correct.

 

F_resultant = (F*(D-d))/D

Where

D= hole diameter

d= tool diameter

F= the normal straight line feed for that tool

 

 

1 Like