Using a thread mill

[Code_Breaker]

Hey, everyone . . .

 

This thread is an answer to a previous thread about getting multipasses using a thread mill. Here is a solution that I worked on that is better than using the thread mill option in MC v9.2 SP2.

 

See example at cadcam’s FTP site in v9 folder call THREAD_MILL.MC9.

 

Using thread mill 1/4-20 OSG Exocard #41000008

 

First step is to create geometry:

 

1. Choose Main Menu ==> Create ==> Next menu ==> Spiral/Helix. The Spiral/Helix dialog box displays.

 

2. Select the Helix operation radio button.

 

3. Enter the parameters as follows:

 

[*]• Starting Angle – Sets the angle at which the helix will begin. (my example 0)

 

• Pitch – Sets the distance from a point on one thread to the corresponding point on the next thread measured parallel to the axis. (my example .050)

 

• Taper Angle – Specifies the thread taper angle. (my example 0)

 

• Radius – Sets the radius for the first spline in the spiral. (my example .250 the major diameter)

 

• Incremental Angle – Controls the number of points on each spline by specifying the angle at which Mastercam will recalculate the spiral. (my example 1.0)

 

• # of revolutions – Sets the number of times the spiral will complete a 360-degree revolution (my example 2)

4. Choose OK. The system calculates and displays the tapered helix in the graphics window,

 

5. Centered on X0, Y0. The Point Entry menu displays.

 

6. Place the helix using the Point Entry menu selections or by clicking the mouse button at the desired location at deepest point of the thread.

 

7. Place two points at center of hole, one at the deepest point of the thread depth to serve as a lead in for cutter compensation. The second at the same level as the top of the helix to serve as a lead out.

 

Second step is to create tool path:

 

1. Main Menu ==> Toolpaths ==> contour ==> chain. Select lead-in point, then spline (at bottom), then lead–out point.

 

2. Select your tool and enter the parameters as follows:

 

[*]• Depth to 0 for 3D contour

 

• Turn off infinite look ahead

 

• Use wear with Lead in/out… parameters sets with both line and arc at 0, and ‘use entry point’ and 'use exit point’ turn on, while all the others are off.

 

•Turn on Multipasses and set your parameters as your heart’s desires. (my example is 4 rough at .013 and i finish at 0)

And you have tool path with cutter compensation and multipasses.

 

 

HTH

Code_Breaker

[Toolfab]

Sounds really cool. Thanks for the tip! I will go look at the file now, but great description!

 

 

[Code_Breaker]

Thanks Toolfab, let me know if you find something I need to tweak. Always looking to impove my work.

 

 

Code_Breaker

[kccadcam]

I've always created a threadmill toolpath just picking a point, then tell it stock to leave,

copy the operation down, less stock to leave and so on until the finish pass. Quick, down, and dirty....

[Fig sign]

I use Contour toolpath to get a thread with threadcutter!

You have multipathes rough /finish and many other things .

See my Dirty tricks examples

[Code_Breaker]

Kevin,

quote:

---

copy the operation down, less stock to leave and so on until the finish pass. Quick, down, and dirty....

---

Not so quick. I've used thread mill and did just what you have described, but copy and change operations depths took too long. I needed a faster method, hence, the method that I described in this post.

 

 

Iskander,

quote:

---

See my Dirty tricks examples

---

+1000

 

 

Code_Breaker

[DavidB]

Does this mean this method has to be done on a machine that knows where the spindle orentation is?

If it does 1 pass then another it would have to start in the place.

 

Maybe M/C can put in spring passes in VX like they did for other types of toolpaths for V9.

 

[Fig sign]

quote:

---

5277

 

posted 03-02-2004 05:08

--------------------------------------------------------------------------------

Does this mean this method has to be done on a machine that knows where the spindle orentation is?

---

No ,it does not

[DavidB]

I will have to think about that then its late and im going home.

 

[jimp]

Hi Code_breaker Thanks for your help it seemed like the answer to my prayers. I am machining a male thread modified Butress 2.5" x 1/8 pitch on quartz, it machines ok but at the end even though i have a start and finish Point it goes straight back to the start of the Helix direct from the end cutting through the thread. (I am cutting top to bottom)

I have the points at the correct depth but only seems to go to the points at the top of helix depth. any help will be very much appreciatedas I have been at this for hours now with no results.

 

JimP

[Code_Breaker]

JimP,

 

Email me the file, and I will look at it.

 

 

Code_Breaker

[jimp]

I have e-mailed you a copy thanks for your help.

 

JimP

[Code_Breaker]

Jim,

 

I have reviewed your file. I do not know why it want to retract and then go to the second point.

 

But , to fix the problem, I deleted the second point, and then under Lead in/out. Under the Exit parameters, I turned on Retract before last move and Adjust end of contour with the extend turned on. I entered a length of 200.

 

This will take your tool of the part (I believe tangent) before retracting and then returning to the initial point.

 

If anyone know why this toolpath retracts before going to the second point, please let us know. Thanks

 

Jim, I will email you the new file. Hope I could be of some help.

 

Code_Breaker

[jimp]

Thanks for your help, last night I added a arc at the bottom of the Helix different route but same answer as yours. but as you say its not ideal way, what is the point of a entry and exit point if it only uses thefirst point?

 

Jimp

[Code_Breaker]

JimP,

 

Actually, it uses both points, but put a retract move before the last point. I am using v9 SP2 mill3. Maybe in the upgrade or vx, this will be changed.

 

Code_Breaker

[jimp]

Thnks for your help ran the program yesterday, and the buttress thread on the Quartz tube turned out great.

[Code_Breaker]

You're welcome . . .

 

I love success stories . . .

 

 

Code_Breaker