milling threads

[Kevin O]

I need to mill thread details in a mold and I have no idea where to begin. the classes I'm taking haven't gotten that far yet, and I need to program this mold yesterday. can anyone please help or point me in the right direction.

the threade are for a blow molded container

 

thank you in advance

[Fig sign]

Kevin !

quote:

---

Thread mill toolpaths create a series of helixes for machining a thread with a thread mill.

 

1. Choose Main Menu, Toolpaths, Next menu, Circ tlpths, Thread mill.

 

2. Select the points and/or circles using the Point Manager menu and choose Done.

 

3. Enter the Thread mill parameters.

 

4. Choose OK. The toolpath is added to the Operations Manager.

 

Notes:

 

¨ You can also create a thread mill toolpath by choosing Toolpaths, Circle paths, Thread mill from the right-click menu of the Operations Manager.

 

¨ If you select duplicate geometry, or if you select a circle and its center point, the duplicate geometry displays in red and a warning displays.

 

¨ The number of active teeth, top of thread, thread depth and thread pitch parameters all indirectly determine the number of revolutions that the tool makes while machining the thread. If the number of revolutions is less than one, the top of thread adjusts to result in at least one revolution.

 

¨ You can create a pipe thread or tapered thread by selecting an appropriate tool and setting the Taper angle parameter in the Thread mill dialog box.

---

There are other ways to do it too ,one of them

is more dangerous a bit way to do threads ,which I use .

It not always works ,so if you satisfied with thread mill toolpath ,no need to talk about it .

If no ,have a look here

 

HTH

ITHH

[Toolfab]

You could check out this Thread also fo some tips.

 

[Kevin O]

Iskander I am grateful for the quick responce

I tried what you suggested earlier but the cutter wouldn't follow the helix it made a few passes in space one pass lightly cutting and one or two deep cuts in a "D" shaped path.

please keep in mind that I am a novice in master cam I have only been trying to program for less than a year (25 years as a designer)

[jrykrl]

Sounds like a lead in, lead out problem.

Check the values for that.

hth

Jer

[Kevin O]

one thing I forgot to mention is that I need a full inturruption of the thread at the parting line. that may be why I'm getting screwy paths.

can I get good thread paths from a solid model?

[Fig sign]

In mcam91millsamplesCircle toolpaths have a look on

THREADMILL-EXTERNAL.MC9 example .

HTH

ITHH

[Fig sign]

You can build a helix and mill it using contour toolpath

Use Create->next page->spiral/helix

quote:

---

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.

 

¨ Pitch – Sets the distance from a point on one thread to the corresponding point on the next thread measured parallel to the axis.

 

¨ Taper Angle – Specifies the thread taper angle.

 

¨ Radius – Sets the radius for the first spline in the spiral.

 

¨ Incremental Angle – Controls the number of points on each spline by specifying the angle at which Mastercam will recalculate the spiral.

 

¨ # of revolutions – Sets the number of times the spiral will complete a 360-degree revolution

 

4. Choose OK. The system calculates and displays the tapered helix in the graphics window, centered on X0, Y0. The Point Entry menu displays.

 

5. Place the helix using the Point Entry menu selections or by clicking the mouse button at the desired location.

---

[Fig sign]

This is my example of milling helix

 

Milling helix

 

HTH

ITHH

[PE @ IHS]

Have you considered making an electrode instead and burning the thread profile? When I worked on blowmolds, we generally burned the threads in.

[Fig sign]

quote:

---

Have you considered making an electrode instead and burning the thread profile? When I worked on blowmolds, we generally burned the threads in.

---

That`s a good idea !

I do it a lot and turning an electrode 180 degrees you will always get perfect parting line .

But you must take a spark into account

[Fig sign]

BTW ,we use EROVA electrode holders .

Great for turning electodes 90,180 degrees ,in dfifferent planes ,quick mounting and so on .

Very accurate but not cheap !

[gcode]

quote:

---

That`s a good idea !

I do it a lot and turning an electrode 180 degrees you will always get perfect parting line .

But you must take a spark into account

 

---

I wish I had a tiny clue what you guys are talking about

 

gcode teh never even seen a blow mold

[Noel]

We do the type of neck insert threads you are talking about alot. We used to do them manualy on a threading table that can be set to rise and ower at the proper pitch for the thread.The head of the bridgport is then tilted to the proper helix angle so to eliminate the wiping efect of the cutter.Once the cutter is set in the x direction it is never moved.The cutter is fed in the y plus direction until the correct dia is reached.then the tabe is rotated the corect # of turns called out on the print. I have figured out how to do it on the nc mill but it is basicaly the same idea.I just use the rotary table to turn the part past the tool using the y axis to control the dia of the thread. I still have to tilt the head to the proper helix angle for each indevidual thread.

 

 

Noel

[Kevin O]

I did the helical contour it followed the helix

pretty well put add a lot of vertical moves that would destroy the part. I've had the problem before, when there's a vertical wall involved the cutter will not follow a smooth path it's like the cutter is trying to climb the wall

[Fig sign]

Kevin !

You probably doing something wrong .

Download from ftp mentioned above in Dirty Tricks example files and have a look .

[Kevin O]

I can't get to the ftp site to download

[Fig sign]

Kevin .

Hold tight

Geometry -helix

Toolpath -contour

Type -3d

Deselect Infinite look ahead and optimize

In lead in lead out deselect entry-exit gouge checking

Imply filtering if your machine can interpolate 3 axes arc movements together in filtering switch on create arcs in XY plane and one way filtering ,give tight value for tollerance and reasonable look ahead.

If your machine can not do sorta g3 x y i j z together deselect create arcs in XY plane .

Now if your backplot works OK ,but in code there are no arcs ,in your post you must switch on support for helix interpolation.

HTH

ITHH

[cadcam]

Sorry guys power was out for me and the ISP now the FTP is up and running.

[Kevin O]

to respond to your suggestion about burning the threads in I agree it would be a lot easier for me

but the powers that be want them either milled or turned and I have absolutly NO idea how to program for a lathe. for that matter how youcan turn an inturrupted thread.

I would like to thank you all for your help and suggestions you have been a great source for information