[jsheerin]

I tired thread milling on my router for the first time yesterday, and it turned out pretty nice. I needed a filler neck for a coolant expansion tank I was building for my motorcycle, and it had some large diameter funky threads on it. I cut them with a 60 degree angle cutter from Enco. The radiator cap fit on them perfectly the first time. Visual Mill didn't handle the thread milling cam generation very well, so I ended up having to write the code for this by hand using Excel. It wasn't very efficient, but it worked. Some pics are attached, and here's a video I took while of the thread milling operation:

[nomedia="http://www.youtube.com/watch?v=ypf9P_qs6X4"]YouTube - Thread milling on my cnc router[/nomedia]

[jimmyaz]

That's pretty cool.. I can't imagine me trying to learn how to write code.. haha... I am wondering if CamBam can do this...

[louieatienza]

I've been meaning to buy some threadmills to test this with OneCNC... would make it a lot easier to make fixture plates... Nice work!

[tkubic]

How did you hand write the code? Just figure out a 3rd order function and then create an array using a small step size?

[jsheerin]

There are maybe 3 G0 and G1 lines that position the cutter and feed in tangentially to the start of the helix. Then there are 3 G2 lines to create the helix (having a Z value to give the change in height from the start of the circle to the end). 1 G2 command for each circle - I needed 2.5 pitches, so 3 lines. Then there are two G1 / G0 lines to feed out of the cut and up to a safe Z. Then repeat that sequence with different values to take the next cut. I set it up in excel and then did some cutting and pasting to get the entire sequence - it just made it easy to keep track of the center point and x/y/z positions for all the incremental cuts. I didn't do anything fancy like a loop.

[jsheerin]

I guess I could add that I also offset the tool path to account for cutter diameter and a Z tool offset (I zeroed the took on the bottom face, but I cared about where the tip of the angle was).

[jsheerin]

Here's what each pass looks like:

X0.414 Y1.2105
Z0.3305
G1 X0.914 F10
G2 Z0.1755 J-1.2105
G2 Z0.0205 J-1.2105
G2 Y-1.2105 Z-0.057 J-1.2105
G1 X0.414
G0 Z0.8305

I varied the dimensions to make the cutter step in on subsequent passes. Then because my thread had a wide land at the bottom of the thread, I had it step down on subsequent passes.

[tkubic]

ahhh, much simpler then i had been thinking.

For one of my machine dynamics courses they had us use excel to create a double dwell cam. We had to determine the functions and then calculate the x,y positions at 200 points which was interpolated in the program.

I feel as though I should pick up a gcode course somewhere to make some cam headaches go away .

[tig-racer]

that is some awesome work. i hope im able to make parts half that nice once i get my system up and running.

[jsheerin]

Yeah, a cam would be more complicated... I took a course where we did some g-code programming in college, but I forgot it all. I have to look up the syntax and figure it out each time I have a problem and have to figure something out. That's why I bought visual mill - to try to make those problems go away. But it seems like I have one every time I try a new feature... I guess I see g-code programming as more tedious than anything else, and if you mess up you might screw up your part or a cutter.

I rode my bike tonight with this part on it and working - for the first time in about 6 months. It was cool. Then I put the body panels back on and noticed an interference on the gear shift lever (a new one), so now I get to make one of those.

[giz]

great work.