Programming acme double lead threads

[KTthunder]

Hi
I'm currently a programmer for my company and I'm straight out of trade school,not to much experience I've been with my company for about eight months and I'm in charge of all the machines in our shafting cell. We have been cutting our 5/8-8 and up acme threads with a die head on a manual lathe after it is machined in a leadwell cnc lathe with a fanuc controll. I'm just trying to better my self for the future and learn and also try to increase productivity with my machines. My question is how would I format these programS to do this? Or would I need special tooling for this?
Any advice would be great
Thanks!

[cadcamwiz]

Several different ways to do this but this should work in your application. Program the normal G76 cycle 2 times and change the Q value 180 on the second cycle

G76X_Z_I_K_D_F_A_P_Q_;
I : Difference of radiuses at threads
K : Height of thread crest (radius)
D : Depth of the first cut (radius)
A : Angle of the tool tip (angle of ridges)
P : Method of cutting
Q: Shift angle of thread cutting start angle

[angelw]

Hi
I'm currently a programmer for my company and I'm straight out of trade school,not to much experience I've been with my company for about eight months and I'm in charge of all the machines in our shafting cell. We have been cutting our 5/8-8 and up acme threads with a die head on a manual lathe after it is machined in a leadwell cnc lathe with a fanuc controll. I'm just trying to better my self for the future and learn and also try to increase productivity with my machines. My question is how would I format these programS to do this? Or would I need special tooling for this?
Any advice would be great
Thanks!

Cutting a multi-start thread is relatively easy. Some controls have an address function to index the thread for the 2nd and any successive leads of the thread being cut, as indicated by cadcamwiz, but what works on all controls is to shift the start point of the threading tool by a distance equal to the thread lead divided by the number of starts.

Take, for example, a two start thread having a lead of 6.0mm. In this case the pitch is 3.0mm. Therefore, to cut the 2nd start, the start point for the threading tool is moved in the Z axis by 3.0mm, either closer to, or further away from the start end of the thread being cut. In all thread cutting involving the treading tool's travel synchronizing with the spindle rotation, there is an area at the start and end of the thread, when the machine slide is accelerating and decelerating respectively, where the lead will be erroneous, and is directly related to the feed per revolution of the slide and the spindle revs. This erroneous lead area is easily overcome at the start of the thread, if the tool is able to start at any distance from the start of the thread, but is more difficult to nullify at the end of the thread if threading to a shoulder. There are formulas to apply to calculate the length of both the acceleration and deceleration error zone. I'm pointing this out, because you must be mindful of this when repositioning the tool's start point for successive thread leads. Generally its better, if space allows (there may be a tail stock in the way) to move the tool further away from the start of the thread, rather than closer to. In this way you won't move the error zone onto the actual start of the thread. In a two start, 3.0mm pitch thread, if the first lead is cut with the tool starting at 6.0mm from the end of the thread, the start point for the second start would be from Z9.0.

In multi-start threads where quite a lot of material is removed to form each lead, if each lead is cut separately, each successive lead will be cut with a cutting tool that has more wear than it had when cutting the previous leads. If a thread gauge is in the form of a screw on GO/NO GO gauge and it won't start, which lead is incorrect? To overcome this, I've created a threading cycle, where one pass is taken successively on each thread lead until finished. In this way, each lead is being cut with a tool having practically the same amount of wear. Accordingly, if the gauge doesn't fit, then all leads are oversize.

Regards,

Bill

[cadcamwiz]

In multi-start threads where quite a lot of material is removed to form each lead, if each lead is cut separately, each successive lead will be cut with a cutting tool that has more wear than it had when cutting the previous leads. If a thread gauge is in the form of a screw on GO/NO GO gauge and it won't start, which lead is incorrect? To overcome this, I've created a threading cycle, where one pass is taken successively on each thread lead until finished. In this way, each lead is being cut with a tool having practically the same amount of wear. Accordingly, if the gauge doesn't fit, then all leads are oversize.

Nice pointer on that Bill. That has bit me in the ars sooo many times. I would cut the thread and gauge would nogo so I wound up buying dies to chase the threads not realizing the simplicity of the problem.

[MLeonard]

To overcome this, I've created a threading cycle, where one pass is taken successively on each thread lead until finished.

Very cool. Would you be willing to share your macro with us?

Balancing the cuts should also reduce, or at least equalize, part deflection. If you cut the first start to full depth before beginning the second start, then the workpiece will not be as rigid when you are cutting the second start.

[gorrilla]

Very cool. Would you be willing to share your macro with us?

Balancing the cuts should also reduce, or at least equalize, part deflection. If you cut the first start to full depth before beginning the second start, then the workpiece will not be as rigid when you are cutting the second start.

My thoughts exactly about the rigidity of the part. Especially if you were cutting something as deep as acme threads. But the balanced approach would solve all that. I'd really be interested in seeing that macro. Not only would it solve the problem at hand, it would further my education about macros, which it needs drastically.

[KTthunder]

I really appreate your guys help on this matter, now I was curious sincer you where talking about tooling wear could it be possible if I used to identicle tools in thee program to for the second thread cycle?

[bhigdog]

Not trying to hijack the thread but after the OP's problem is solved whats the procedure for single point cutting a double lead screw on a manual lathe...........Bob

[angelw]

I really appreate your guys help on this matter, now I was curious sincer you where talking about tooling wear could it be possible if I used to identicle tools in thee program to for the second thread cycle?

You can use as many tools as you like in any type of operation. However, in the case of your part, the cycles for cutting the two thread leads will be in the one program. If the you were cutting an acme thread, for example, having a relatively large lead, and therefore a relatively large thread height, you could use one tool each to rough each start, and then a third tool to take a finish pass or two on each pass if your were concerned about tool wear.

Very cool. Would you be willing to share your macro with us?

Yes. Give me a day or two to get it off of a machine, or find it on a computer.

The following block is the Macro call block. I was able to output that from my CAM system that's on this computer, but the actual Macro program lives in the control that uses this function.

A custom G code was created, thats Greasy Kids Stuff, you can register any number you like, but G176 made sense to me, as its a step up from G76.

As you can see, the G176 block uses the same arguments as the standard G76 (Series 15 Format), with an additional Q address for the number of Thread Leads, and M for the minimum depth of cut

G176 X22.0 Z-50.0 K2.0 D0.5 F6.0 A60.0 Q2.0 M0.05

Regards,

Bill