3d bass relief - how do drill with endmill

[wodkreso]

Hi. I have small CNC doing aluminium mostly, and recently I started doing some 3d machining with it.

I tried several programs to generate toolpaths for me, and in all cases they "easily cold blooded" go and drill holes with my endmills - at least to enter depth they need.

However, I use proxxon 3mm endmill which doesn't behave nicely when asked to drill a hole - not even small as 0.3mm. I just can't believe I should replace tools (manually) all the time to put real drill inside for a small hole.

I understand endmill needs to enter somehow to required depth - but most of those softwares go "up and down" on various places drilling new holes when on other side of the same layer there is already hole made from previous cut. I've read other threads that endmills are not made for drills - and I have similar experiences.

So am I missing something - if endmill cannot drill required depth, why do softwares (such as Cut3d or meshcam I made most tests with) don't try to minimize drilling to required depth and then re-use the hole previously made? Or, is there some other standard procedure for going deeper into the stock with endmill? I hope I don't have to replace tools all the time since per layer sometimes it's 20 times, and my layers are 0.3mm in depth, total 5cm deep to cut (so, it's like 150 replacements).

Thanks for any insights!

Kreso

[keebler303]

You want to used ramped plunges. Any decent CAM software should at least have that option. That way it is going sideways as it goes down to minimize cutting with the bottom of the endmill.

Matt

[wodkreso]

Matt,

thanks for your reply. Can you suggest some software that is not professionally expensive, and can be used by hobbists?

BTW this "ramped plunges" is this same as "helical paths" that I've read in similar posts?

Thanks!
Kreso

[keebler303]

A helical path is a ramped plunge with a circular path. A helical path has the shape of a helix, a ramped plunge has any arbitrary path in x,y with a steady plunge in z.

I use artcam, I think it may be above your budget, I am not the best person to comment on the lower end softwares, as I have never used them. Maybe search the forum for some threads about it.

Matt

[Russ Kaiser]

Kreso,

I use MeshCam exclusively for 3D work and I am having trouble understanding your issue. MeshCam should never be asking your mill to plunge more than your cut depth. The program may choose a different starting position for each pass, since it is trying to optimize and limit unnecessary rapids, but the material in that location should have been removed in the previous layer. So if you have a depth of cut set to 0.3mm, that is the most you should ever see your mill "Drilling"

The speed at which you plunge in MeshCam is a separate parameter and for aluminum, this should be very slow. I typically run 2 to 3 inches per minute for plunge speed.

Also, you should be using 2 flute mills designed for bottom cutting. Some 2 flute and most 4 flute mills will not drill well. Suitable mills are available even in the tiniest sizes. I have bought several small mills from American Carbide that are capable of drilling the start of each pass.

Also, I typically run multiple roughing passes using smaller and smaller tools. Get most of the material out of the way with larger, sturdier mills and then go for the detail work using the small stuff.

I hope that helps,

Russ