Thread Milling with Sprutcam 7

[Tbkahuna]

I have gone over the sprutcam tutorial at Tormach and searched here and didn't find enough information to help with setting up thread milling in Sprutcam.

I have a round part of say 1" diameter that is machined to .75" diameter for .75" on the end. I want to thread mill 3/4" x 16 threads from the end down .657".

I used 2D contouring to reduce the diameter to .75". My model has a .673" diameter (minor diameter of the 3/4" x16 external threads), so I left the extra stock as part of the 2D contouring operation done right before I try to do the thread milling of that section. I built the model with a .673" diameter after watching the Tormach threadmilling tutorial where they use the minimum diameter and then add stock to the model so you can watch it get cut away in simulation.

In that tutorial, it also interferes with the model as it cuts the full length of the surface. I only want to cut threads down to .657" from the end, not the full .75" length. I selected one half of that face and the "Center" command for the job assignment. I then adjusted the Z dimensions of the hole to 0 for the top, and -.657" for the bottom. The job assignment looks to be correct and doesn't show the full .75" depth.

I am using a 1/2" single point thread mill, built as per the Tormach tutorial. The bottom half is the tool, and the rest is the holder. Has any one used any other method for creating the tool or defining the thread milling tool path?

So far, so good, but when I generate the tool path for the simulation, I get a 10 second estimated time and absolutely no simulation runs for the thread milling. Any ideas on what I need to do?

This is the only code it is generating:

N2980 M5 (Inch)
(Hole machining 5D)
N2990 M998
N3000 T20 G43 H20 M6
(Thread Mill Carbide 16 - 20 TPI)
N3010 S650 M3
N3020 G0 X0. Y0. Z9.387
N3030 G0 M998 M5
N3040 M5 M9
N3050 M30

Thanks for any help.

[saabaero]

I had done thread milling on my Tormach once in the past. It was for a left hand 16mm x 1.0mm thread in hardened stainless steel using a carbide thread mill. I wanted a tight fit to an existing (female) part so I selected a 2D contouring machining operation with cutter diameter compensation. In the "strategy" tab I set "Helical machining" to "Available" and in the "Parameters" I set the "Depth of Cut" to 1mm and a "Bottom Level" to 16mm (the length of the thread I wanted). By using "cutter diameter compensation" I was able to run the same program while varying the cutter diameter to get the fit I wanted. By inputting a cutter diameter (into the Tormach tool table) smaller than the actual cutter diameter (and working down in size) this allowed me to mill to the "minor diameter" I needed. You can calculate this if you just wanted to make one pass.

If you wanted to make multiple cuts to get to your final minor diameter you can set the "Roughing Step Parameters" in the "Strategy" tab to cut the thread in the depth increments you want.

I wasn't quit sure of the quality of the thread I would get at first but was extremely pleased with the result. I got a smooth, tight fit to the existing part. The part was a nozzle for a high pressure waterjet cutter (60,000 psi)

The code resembled:
...
G21 (Metric)
(2D Contouring)
M998
T35 G43 H35 M6
(0.500" thread mill)
S3500 M3
G0 X24. Y0. Z5. ('compensation switch out' lead in for cutter comp.)
G42 (turn cutter comp. on)
G1 Z0. F100 M8
X8.
G3 X8 Y0 Z-1. I-7.99999 J0.00001 F200 (start 1mm above part)
X8 Y0 Z-1. I-7.99999 J0.00001 (repeated 16 more times while "Z" increments 1mm each time)
...
G1 X24. ('compensation switch out' lead out for cutter comp.)
G0 Z1.
G40 (turn cutter comp. off)
......

I'm sure there are a half dozen ways to accomplish the same task in Sprutcam.

[TDukes]

Did you ever come up with a solution?

I am currently trying to learn to use SprutCAM and I am attempting to try thread milling with a double angle cutter as described and setup using the Tormach tutorial video. If I use the cutter setup with the exact parameters described in the tutorial it works. However, when I change the cutter size to the size I have it will no longer work. It is a 0.75 diameter double angle cutter with 60 angle. Height .1875 when I put the following parameters in the tool table L=0.09375, D=0.75, a=60, H=0.09375 and for the holder I have 0.75:0:0.375:0.09375:0.375:1 it draws the cutter properly. Unfortunately it will not work or generate the code. If I play with the numbers and make the diameter 0.5 or less it will work unfortunately the only cutter I have found or have is 0.75. Any suggestions as to what I may be doing wrong?

Thanks in advance,
Todd

[Tbkahuna]

No direct solution for me. Saabaero explained his method. I got tired of messing around with it and just used the Mach 3 and then New Fangled Solutions thread milling wizards. They both worked pretty well for what I needed. However, there is an automatic move at the end that caused tool/part interference. I was threadmilling from the bottom of the thread up, so I just let it make a couple more revolutions after it was out of the steel, so the move was done safely "in the air".

Here shortly I am going to get a multi-form tool and just set up my standard block of code (since it will be much shorter) for it and insert it into my programs as needed.

[saabaero]

In the case of Sprutcam not generating a toolpath... Just a quick guess, without seeing the project... would be to make sure the tool is cutting material. Most times Sprutcam doesn't generate a toolpath it is because there is no stock to remove and the tool would just be cutting air. An adjustment to a parameter usually solved the problem

[dkaustin]

tbkahuna--

I was having the same grief as you. Couldn't get the thread milling simulation to run to save my life, even though I set it up as per the Tormach tutorial.

Then I checked the one thing the tutorial didn't address.

Go to Machining>Work Assignment and right-click to see the hole properties. I had to input these values manually, and --voila!-- the simulation started working. "D" is the diameter of the thread mill cutter. Zmin, Zmax, and H are determined by the length of the threaded section.

Of course, SprutCAM insists that my workpiece is a box instead of a cylinder, but that's another problem. :-)

Hope this helps!

[TDukes]

That did the trick - Thanks

[dkaustin]

Ooops. "D" is the major diameter of the thread, not the diameter of the thread cutter.