Internal Rope Thread>>>>>>>>>Made it Work

[Mr. Wizzard]

Yeah, it's been a while.

So I have something i've never come across before, ROPE THREADS.

Specifically: ROCK DRILLING EQUIPMENT - LEFT HAND ROPE THREADS.

I'm not yelling just emphasizing the particular information I have. I don't know what size I'm going to have to do yet, but they will be internal on a 2-axis lathe. Can anyone help me with figuring out how to do this with Mastercam, or if it's even possible?

Thanks!

[K2csq7]

Custom insert?

Let us know how you get it. Looks tricky!

[K2csq7]

http://www.cenic.fi/english/ropecam_eng.htm

[MMI Robert]

I wish I could be of more help than this. I had to look up a "rope Thread" first looking at drilling pipe thread geometry then doing a search on the net. I found a u-tube video of an external rope thread being cut on an Okuma lathe with a single point insert. They were using a technique refered to as cam mode or cam cycle. I hope watching that will give you some ideas.

[Greg Williams]

Your only choices on a 2 axis lathe are a custom insert, which may not work due to the large cutting area or some funky code from specialist software.

[MMI Robert]

This may sound crazy but.. Surface it with a round insert and multiple passes. This is a technique which will take a fair amount of time, but if this job is a must do it will work. Be cautous because there are a mess of gotchas in it.

 

We are going to create a mill surfacing tool path to get the points. Isolate the geometry of one full pitch at the Y location of tool contact. Move to seperate level. Copy the geometry .5 inch or what ever from the location of the first. Create a surface between the two. Orient planes for a standard xyz mill pass. Select a ball mill the same size rad as your turning insert. Generate a surfacing tool path, perhaps flowline. Modify your post to swap z/y etc so that the code will have the same axis designation as your lathe. Post. You will ignore all long linear movement and delete. What is left are y & z positions. Use these positions to set your y and z lathe start positions. The pitch will be controlled by your feed rate. Be careful to start out away from your part z0 the tool start position will change as you progress through the program. Thread termination is dependent on whether this is a thru thread or there is thread relief. Remember all you really need are the points. I would remove as much material as possible before going after the actual thread formation. Good luck.

[Mr. Wizzard]

Keith, thanks, but I don't think another software is an option right now. It does look like the way to go, but this may be a one off thing. I don't have a lot of information on the job yet.

 

Robert, wow. That sounds amazingly complex. I'm sure we'll have to go with a round button style insert, but i don't how to approach it just yet. I'll keep you posted on my progress. Please do the same and hopefully we can help out anyone else that may come across this.

 

Thanks guys, i'll let you know.

[K2csq7]

Keith, thanks, but I don't think another software is an option right now.

 

I was just really surprised to find that there is actually a software package designed to do that!

Getting the bottom (root) of the thread with a full rad insert is the easy part.

Maybe you can take the threading path for the bottom of the thread and shift it up in X (dia) (then back down after the top of the arc) and deeper in Z, making your own stepover kinda thing.

The only worry I would have is how to keep "top dead center" on your lathe. If you have the ability on your lathe to "pick up" thread start points and you are fluent in how to use the function you should be able to get it done with some trial and error.

[MMI Robert]

Mr. Wizard A problem or solution is only complex until you break it down into it's componant parts. The parts are generally manageable.

[RayD]

Thread-C Chook?

 

Although I have never tried it, but it could in theory work.

 

I have cut them manually programing with a button insert for the root, and I Profiled the OD/ID Shape with VNMG.

[GoetzInd]

Maybe something like creating a finish pass of one full form, turn off arcs (set accuracy to what you can live with surface finish wise), and use those as start point in G32 passes with the pitch of the rope thread.

HTH

 

Mike

[Mr. Wizzard]

Mildly time consuming, but i think i nailed it. May need to tweak, but that's why i'm The Wizzard!

I'll share details later.

 

RayD, sound like a good thing to try. I may look into it later just to see if there's a better way. Definitely a good idea, though.

[GoetzInd]

I've got your problem solved! Just call OKUMA!

 

[Mr. Wizzard]

Regular 2-axis lathe.

.313 wide full radius insert

I did my test part on the OD, so i could see what was going on.

Here's the process;

1- create the geo, surface optional, but i like the visual

2- offset the chain .1565 (radius of the insert)

3- create spline from curves, chain offset geo

4- break spline (picked .025 segments)

5- create points at segments (ended up with 22 points for 1 pitch)

6- create threading toolpath, select first point for "minor diameter & z start point", comp tool to center of insert

7- copy toolpath 21 times, change minor diameter & z start point to each of the other points in succession

8- post so you get G32 cycle at each start point

9- set up tool and increment your "Z offset" +.1565 and your "diameter offset" -.313 to bring the tool tip to the finish geo

10- run part and be amazed

 

I need to tweak some things in, maybe smaller steps and multi-passes, but overall i'm satisfied with the first trial

[sergn]

I want to offer a method of rope threading wich reduce the cost of manufacturing rope thread in rock drill tools.

Processing takes place on a milling machine with CNC. Cutting speed=200m/min, fedrate 0,03 mm/tooth (190 mm/min), tool may have more than two teeth.

Tool use required standard cutting inserts, for example: WALTER: CCMT060204-PS5 WPP20.

http://youtu.be/0JsVJskwQ-g

[Ron Poulose]

Hi all, 

 

one of my concerns on this with which any one of you can help me out with

 

 

I have cut the external rope thread on an rod and has come out good using a DNMG 1.2, my concern is whether this would work on the internal threading aswell? If not which insert and tool holder can we use for the same? 

 

 

thanks in advance