4th axis carving questions

Hobbyist level, I have built 3D printers and refurbished an old Epilog Laser, Now I am looking at building a task specific 4 axis router for gun stocks.

I have seen what appears to be 2 distinct styles of carving a gun stock on a 4 axis router.

one has the 4th axis just "indexing" the stock and the tool carving Longitudinal as shown in this video: https://www.youtube.com/watch?v=P5_nT1hsQf8

The other is where the stock continually rotates on the 4th axis as it is carved "Radially" https://www.youtube.com/watch?v=Ik_UKwVTMv8

Questions:

Is one method better than the other?
Does it require different CAM packages to perform one or the other?
What would be a good "Hobbyist" CAM package to perform one, the other, or both?

It looks like they are using a Ball end bit for their carving, for the final cut it would seem the point of contact/cut would be infinitely small, requiring the passes to be in the millions for a smooth finish without ridges?

I have found books and articles explaining generic CNC router theories, but nothing in depth dealing with 4th axis, bit choice and carve paths for desired results,, Does anyone have a good source for reading material for these subjects,

Many Thanks,
Slack

The choice of which 4th axis carving strategy to use - indexing or continuous - depends on the configuration of your part and your expectations for it. To use your rifle stock as an example, if that slot in the top of it needs to be square on the sides, then an indexing strategy would be best. If you carved it using a routine where the tool moves down the X axis, increments in A, then moves back up to X zero, etc. then your slot would be wider at the bottom than at the top. But if your primary concern was smoothness on the outside, you could use the continuous strategy and put in the slot later, as a separate operation. Indexing usually will show a little discontinuity where the various toolpaths meet.

For jobs like this where you need a smooth contoured surface, a ball-end tool is always used. Otherwise you'd have gouging from the edges of a flat endmill. It does remove less material at a time, though. 3D carving is always going to be slower than 2.5D. The cusps where the passes of the tool adjoin are smallest when the diameter of the tool are largest and more noticeable when the diameter is smaller. To counter that tendency, you need to space the step-over tighter with smaller tools. But it's not in the millions even then; an approximately flat surface can be achieved without infinitely small step-overs. Since your rifle stock has a generally smooth surface without tight spaces that need to be reached by the tool, it looks like you could do the whole thing with a fairly large-diameter ball-end cutter, like about half an inch.

I'd suggest using DeskProto as your CAM package; it can do both types of 4th axis carving - indexed ("n-sided") and continuous (along X or along Y), and has a lot of other handy features as well. We sell the multi-axis edition at a significant discount to hobbyists. I don't know of any books that talk about 4-axis carving in any depth, but there's a lot of instructional material on the DeskProto site: DeskProto offers CNC machining for non-machinists

Thank you for your in depth response.
The inlay would be a separate operation, most likely with a bit change to an end mill bit.

I will look into Deskproto and the associated literature.

You may find that you get a better finish machining along the stock, with the grain of the wood. But you may also finds that it's more susceptible to tearout that way, depending on the roughing strategy.

There are very few CAM programs that support continuous 4th axis. The "Radial" method. I think Fusion 360 offers it in it's machining extension, for an additional $1600/year.

Gerry,
Thank you for the response, 90% of what I use would be laminated plywood.
What is odd is both videos are from the same machine supplier,, unsure of why they used different techniques.
I may give them a call and see if they will give a "Hobbyist" 10 minutes on the phone.

Slack

Working on specs for this machine, specifically rough routing plywood that is made with 1/16 colored birch layups, the blanks would be roughly 2" thick.
Before I can think about X, Y, and Z speeds (motor size, type, speed,, screw type/pitch), I need to define what type of bit I am using for this plywood, spindle speed, and HP and type cut depth.

I am hitting dead end finding any reading material specifically geared toward what works, and what does not. I need to nail down my spindle motor and bit before I can continue on the design of the rest of the machine.

Any pointers on lititure?

Thanks,
Slack

First question I'd ask is; what specifically is the make up of the laminated blanks? I've machined laminated knife handle stock (birch as well) and that is a very different animal from plywood. My material was phenolic impregnated and was miserable to cut (smelled terrible and weighed a ton too). That alone warrants special tooling and feed speeds.

Generally, on 3D stuff in hardwoods I start with an up shear corrugated roughing bit often cutting across the grain with perhaps 1/16" stock to leave. Follow that with up or down shear finishing bits cutting with the grain (sometimes climb cut with a follow up conventional cut). This was done with an 8HP spindle run at 16,000 RPM, 3/4" dia bits at 150 to 200 IPM. 60% tool stepover and 1/2" DOC (depending on 1st pass or follow up cuts). These values could be scaled to lesser HP and tooling diameters.

Quality of cut (regarding blow outs and such) will depend heavily on your tool path sequencing choices. Have fun!

I'll agree that a serrated roughing bit is the best choice for roughing. They are awesome, but expensive.
How rigid the material is while clamped to the 4th axis will have a huge influence on how fast and deep you can cut it. You won't really be able to cut fast or deep enough to need any more than a 2Kw-3Kw spindle. This is a fairly light duty application as far as the spindle goes.

Marv,
Thanks for your response. The "plywood" is Spectra-ply, it is 1/16" dyed plys, but they do not spec the resin used. https://www.cwp-usa.com/collections/...l-10x35?page=1

*8HP? that is a heck of a spindle. 3 phase?
I was looking at 3/8" collet and bits to rough out a gun stock. "Hoping" to stay with a 115v spindle,, but wondering if I have to go to 220v single phase.
I dont need "high speed production", but also do not want to grow old waiting on a gun stock to rough out.
But honestly am in the dark on spindles/routers and figured I need to nail down what I need before zeroing in on X and Y travel speeds.

Thanks again,
Slack

Quote:

---

Originally Posted by MARV

First question I'd ask is; what specifically is the make up of the laminated blanks? I've machined laminated knife handle stock (birch as well) and that is a very different animal from plywood. My material was phenolic impregnated and was miserable to cut (smelled terrible and weighed a ton too). That alone warrants special tooling and feed speeds.

Generally, on 3D stuff in hardwoods I start with an up shear corrugated roughing bit often cutting across the grain with perhaps 1/16" stock to leave. Follow that with up or down shear finishing bits cutting with the grain (sometimes climb cut with a follow up conventional cut). This was done with an 8HP spindle run at 16,000 RPM, 3/4" dia bits at 150 to 200 IPM. 60% tool stepover and 1/2" DOC (depending on 1st pass or follow up cuts). These values could be scaled to lesser HP and tooling diameters.

Quality of cut (regarding blow outs and such) will depend heavily on your tool path sequencing choices. Have fun!

---

Gerry,
Thanks for the reply.

Yes, in the relm of things a gun stock is not a large amount of carving, And while I do not want to fall asleep carving a stock, I do not have to squeeze the last 10% of speed out as this is more hobby than business.
2-3KW is what I needed to hear,, now I have a starting point. I do not want a spindle that is heavier than needed, then having to over build the gantry, X-Y drive, etc.
I have no problem spending on a good bit,, but do not want to burn it with to fast/slow spindle speed, or travel speeds.

So 2-3KW spindle gives me a starting point, assuming I will try on the the Chinese VSD units.
Now I just need to figure spindle speeds and travel speeds of the X and Y,, then I can figure how rigid the gantry (how heavy) has to be, and what size steppers/rails.

Thanks,
Slack

Quote:

---

Originally Posted by ger21

I'll agree that a serrated roughing bit is the best choice for roughing. They are awesome, but expensive.
How rigid the material is while clamped to the 4th axis will have a huge influence on how fast and deep you can cut it. You won't really be able to cut fast or deep enough to need any more than a 2Kw-3Kw spindle. This is a fairly light duty application as far as the spindle goes.

---

Just looked at the link to source of material; interesting stuff. Probable not much different from material I've cut. As you probably know, with lower HP an adjustment in feed speed and stock removed is needed, but not impossible. And the tooling I mentioned is also available in smaller sizes. I believe I have a 3/8" diameter corrugated up shear that will work in a 2.2 KW spindle and not that expensive (maybe $50). The nature of the cutting geometry also uses less power to cut. Be sure to post some images of your work when you have your machine up and running.

Once again, Thanks for all your help.
I will post up when this gets going,, probobly 6 months out.

Slack

Quote:

---

Originally Posted by MARV

Just looked at the link to source of material; interesting stuff. Probable not much different from material I've cut. As you probably know, with lower HP an adjustment in feed speed and stock removed is needed, but not impossible. And the tooling I mentioned is also available in smaller sizes. I believe I have a 3/8" diameter corrugated up shear that will work in a 2.2 KW spindle and not that expensive (maybe $50). The nature of the cutting geometry also uses less power to cut. Be sure to post some images of your work when you have your machine up and running.

---