[kvom]

Isn't CamBam for milling only? It's also rather limited, in that it only allows one tool per job.

If you already have VisualMill, you'd be well off to learn how to use it. For milling, SheetCAM is very easy to learn, and inexpensive. I think Dolphin is about the cheapest reasonable CAD/CAM for lathe work. You can use the free version of LazyCAM for lathe - LazyTurn (comes with Mach3), but I've always found it to be REALLY squirrelly.

Regards,
Ray L.

Not sure where you got your info, but CB allows any number of tools and generates standard Tn and M6 control words for mach3 tool changes.

CB does have a simple lathe module for turning, but it primarily for milling. There is an active support forum and tutorials, and the product is being actively enhanced.

I had gotten BobCad with the mill, but found the CAM portion unintuitive. CB is much close in design philosophy to MasterCam from school. That said, any CAM program that generates good g-code is fine if it works for you. Since OP has done hand coding and understands g-code, it will be quite easy for him to move to CAM.

[SCzEngrgGroup]

Not sure where you got your info, but CB allows any number of tools and generates standard Tn and M6 control words for mach3 tool changes.

CB does have a simple lathe module for turning, but it primarily for milling. There is an active support forum and tutorials, and the product is being actively enhanced.

I had gotten BobCad with the mill, but found the CAM portion unintuitive. CB is much close in design philosophy to MasterCam from school. That said, any CAM program that generates good g-code is fine if it works for you. Since OP has done hand coding and understands g-code, it will be quite easy for him to move to CAM.

I must be remembering some other CAM I "interviewed" some time ago. I do recall trying CAMBAM several times, and each time finding some serious limitation (for me, at least), but I can't recall what it was. Cam is pretty "personal" - What works well for you, could be awful for me, and vice-versa. Best thing to do is try out several, and see what works for you.

Regards,
Ray L.

[CROSSHATCH]

I'm hoping to do the same thing on the future purchase of the Torus Pro.

I have the lathe but perhaps this might be the route to go for a small run on components.

Good stuff!

-Jason

[UniqueMachining]

It's been awhile since I have posted any activity. I finally decided to buckle under and learn Visual Mill CAM. With the much appreciated assistance of another user and Team Viewer, I have managed to grasp the basics. Back to the Pulsar ("My Temporary Mini Hass Tonka Toy").

Having way too much fun, as I continue to push it. As I get more comfortable, I am utilizing zero-divides feeds and speeds to utilize the beasty to its full potential. (Still some to go).

I completed the programming for the 4 Quick Change Tool Holder for Mill-Turn. The first step, 12- 5.1(.2008") holes (carbide bit), .5 Deep, peck .1, speed 4500, feed 20 IPM went flawlessly. This is double the feed and 1.5 x the speed of the first video. Wonder how much more I can push it?

The second step was a series of .25 holes 1.75 deep. As I don't have a carbide bit that long , I used a long cobalt bit. At a depth of 1.375, despite pecking and lots of flood coolant, it totally clogged. I have decided to drill to 1" with the carbide bit, then switch to the cobalt bit and try two .375 deep cycles with a full retract & dwell between each.

In the meantime I uploaded a video of the first step. Recently acquired a Web Cam with a five times zoom enabling me to mount it out of coolant spray. Future videos should be much clearer.

FYI, for a separate job, I rigid tapped a series of 3/8-16 holes without the slightest strain.

John

4 QC TH Step 1 - YouTube

[photomankc]

This has been a very informative thread. I was going to look into the model with steppers but I think I'd rather just go for the servos out of the gate. Time to start saving up!

[UniqueMachining]

This has been a very informative thread. I was going to look into the model with strippers but I think I'd rather just go for the servos out of the gate. Time to start saving up!

.

If it comes with "strippers" ( I assume three), you best place your order quickly. I'm thinking backorders galore. LOL.

John

[photomankc]

LOL, Then the savings would need to include a divorce lawyer. Damn auto-correct!

[UniqueMachining]

Continuing saga of the 4 QC Tool Holder Step 2 to 5 (Side Only)

Still encountering issues with deep drilling (over 1.25") using cobalt bits. The flutes constantly jam up with swarf. Strangely, the carbide bits don't seem to suffer the same fate. Anyhow, re-programmed the deep drilling routine to three steps.
1. Peck: 0.1", Feed: 20 IPM, DOC: 1", Dwell: 4 sec.
2. Peck: 0.75" Feed: 15 IPM, DOC: 1.375" Dwell: 4 Sec. for (14/-20) holes
3. Peck: 0.50" Feed: 10 IPM, DOC: 1.75" ( 2 Holes for Hex Key Storage)
Seems to have solved the problem.
Posted a video of the remainder of the side operations.
Still have the top to cut.

The first couple of holes in step 2 were pre-drilled prior to videoing. Web cam stopped working and I had to re-start.


4 QC TH Step 2 5 - YouTube

[photomankc]

Watching it tap those holes makes me jealous.

[rlockwood]

Drilling Deep Holes On A VMC : Modern Machine Shop

should give this a read; i'd suggest doing using a deep-drilling peck cycle (g83) to clear the chips.

[UniqueMachining]

Drilling Deep Holes On A VMC : Modern Machine Shop

should give this a read; i'd suggest doing using a deep-drilling peck cycle (g83) to clear the chips.

rlockwood

Appreciate the link. I had been intentionally avoiding G83 because of the full retract after each peck.
My thought was to combine the best of G73 & G83.
I wrote a variable driven subroutine with excellent results for a CNC lathe. Bit of difference though, due to bit orientation & non rotating tool.
Think I will do some more experimentation and time the various results.

Thanks, John

[rlockwood]

I'm fairly sure I had come up with a method to use the two (g73/g83) in sequence, but am having trouble remembering how I got g83 to fully retract, but to begin drilling where the g73 had left off.

Depending on what software you're using and how it passes variables to the post processor; I have some code somewhere to do a subroutine much as you mentioned; it could likely be adapted. Its important that post processor be able to determine the drill diameter, as it uses that to figure out when to switch cycle types.

[UniqueMachining]

This is the subroutine I used to drill 1.75" deep with the 1/4" bit shown in the video.

Will experiment some more & tweak as required.

John

(================================================= ============================)
( * Subroutine to Peck Drill Hex Key Storage Holes * )
(================================================= ============================)
o3200
G90 G99 ( Absolute )
G73 Z-1.0 P0.1 Q0.1 R.1 L1 F20 ( Initial Peck Drill to 1" Depth )
G4 P4 ( Dwell 4 Sec. at Z0.1 )
G0 Z-0.990 ( Plunge .990 Into 1" Pre Drilled Hole )
G73 Z-1.375 P0.1 Q0.075 R-.990 L1 F15 ( Peck Drill 1.0 to 1.375" Deep )
G0 Z0.1 ( Z to Start Position .1 Above )
G4 P4 ( Dwell 4 Sec. at Z0.1 )
G0 Z-1.365 ( Plunge 1.365 Into 1.375" Pre Drilled Hole )
G73 Z-1.75 P0.1 Q0.05 R-1.365 L1 F10 ( Peck Drill 1.375 to 1.75" Deep )
G0 Z0.1 ( Z to Start Position .1 Above )
M99
(================================================= ============================)

[UniqueMachining]

Top of 4 Quick Change Tool Holder Step 7-8

Well, it seems the following routine for deep drilling eliminates swarf buildup on the bit..

Step 7:
Drill 14- 7/16" Holes 1.65" Deep
Speed: 3000
DOC......Peck....Feed (IPM)
0.8"........0.1 .......10
Dwell 2 sec. at Z0.1
1.2"........0.75......7.5
Dwell 2 sec. at Z0.1
1.65.......05..........5

While it is difficult to see in the video, huge stringers were being fired at the enclosure. The size can be seen laying in the tray.

Step 8"
Slot previously drilled 7/16" holes, using 3/4" EM.
Speed: 4500
DOC: .025 (Ramp)
Feed 20 IPM

You will note some holes are partially drilled or milled. The web cam kept seizing up and I had to re-start numerous times. I decided to leave the last two slots and program them as circular interpolation for comparison purposes. Next video.
At the end of the video I included a clip of hosing down the table and trays with the separate spray hose. Very neat, fast and convenient. Also included a clip of the coolant filter after dumping the chips. There is also a second filter on top of the coolant container just in case. I haven't had a single coolant nozzle clog up due do chips in the coolant.

See attached video of the job.

John

4 QC TH Step 4 8 Cleanup - YouTube

[UniqueMachining]

Last time I ended saying that the final 2 pockets for the 4 QC Tool Holder would be machined using cam pocketing. After trying every conceivable option, it turns out that Visual Mill is unable to continuously ramp into a pocket. The only option is to ramp in then plunge to each level thereafter. Just hate the sound it makes and can only guess at the load it places on the tool and machine.

I decided to role my own and wrote a subroutine to ramp down .025" over each full revolution. It just seems to make sense that maintaining an even, constant a pressure on the tool, will significantly lengthen its life. Attached is a brief video test of a full pocket.
Originally the ramp was set to .034" as the pocket on the holder is pre-drilled with 3-7/16" holes to provide for chip evacuation and reduce the amount of material to be removed. As the test pocket had no pre-drilled holes, I backed it down a tad.

The video starts at 20 IPM, increases to 30 and reduces to 10 for the final two finish passes. Got a little worried for the last 3/8" as the coolant flow was no longer aimed inside the pocket. Fortunately all ended well. The results were most acceptable. See individual pics. Based on the sound of the cut, it was not straining at all.

1.5" Deep Hole Pocket
Speed: 4500 RPM
Tool: 3/8" FEM HSS
Feed: 30 IPM
DOC: .25 (Continuous Ramp)
TDOC: 1.5"

John
Deep Pocket 1 - YouTube

[AiR_GuNNeR]

John,
IIRC, in Visual Mill, there is a check box to apply your entry and exit selection to all levels. It's at the lower left of the window.
Eric

[UniqueMachining]

Eric

I had tried and discounted that option for two reasons:
1. It fully retracts and the re-ramps rather than providing continuous ramping.
2. Due to the number of steps involved, it imposes a serious time penalty.
e.g. A sample 6 minute job, turned into 26 min.

Appreciate the tip.

John

[AiR_GuNNeR]

Eric

I had tried and discounted that option for two reasons:
1. It fully retracts and the re-ramps rather than providing continuous ramping.
2. Due to the number of steps involved, it imposes a serious time penalty.
e.g. A sample 6 minute job, turned into 26 min.

Appreciate the tip.

John

I think I see now what you are trying to perform. You want a continuous spiral cut downward. There is a way to do this, but it is not a straight forwared option. You set your cut depth to cut in one pass. You set your entry ramp to a shallow angle, like 1 degree, and set the ramp depth to full depth. You will need to play a little bit with the ramp angle to get the DOC per pass appropriate, but it's pretty quick to do. Basically, this turns your entry ramp into the cut itself.
Eric

[UniqueMachining]

Eric

Tricky Dickie. Sounds like a sneaky out of the box solution.
I like it.
Will experiment and post results.

Thanks again.

John

[UniqueMachining]

Eric

No joy. VM appears not to honour the entry angle which I set as low as .001 degree.
I'm guessing that a entry/exit ramp can only be one move.
I tried various combinations of entry depth at full depth and, various angles but they resulted in plunging to full depth minus a bit.

Have you ever done it and if so might you have a sample?

John