Mplmaster mod Question (Siemens Threading)

[nofalloff]

Over the last several months I’ve been learning what I could about posts by tweaking all the posts we have in the shop. I also set out to modify mplmaster to work with an old turning center that no one uses, so that when I had small production jobs I could set them up on this machine without tying up any of the others. The machine has an old Siemens 810T GA1 control and I have mplmaster pretty much where I need it except for one last thing.

Threading.

The code for threading for this control looks like this:

N10 R20=.0769R21=.4167R22=.05R23=1R24=-.0416R25=0R26=.05R27=.05

N20 R28=3R29=0R31=.4167R32=-1.1

N30L97P1

 

The L97 is the call for the threading cycle P is the number of times to run the cycle and R20 thru R32 are the thread parameters.

 

I don’t even know where to begin to get mplmaster to output threading in this format. I see the threading variables but I don’t see where they are assigned value or where they are processes or formatted for output (save for “write to current tool record” block[?]).

 

Can anyone help me understand this?

 

I’m not against programming threading by hand but it would be nice to complete this post so that it was truly post and go.

 

thanks

 

peter

working WAY too late.

[crazy^millman]

Well the best way will be to post up what each R value is. Then look to what a standard caned cycle output. Then where each varaible is make them the correct RXX value you need.

 

A format statement would look like this:

fmt R32= 16 thddepth$ #Thread height absolute

 

So when you post out the standard thread cycle you get what you were getting just now in a format you need for the control to understand. Pretty straight forward.

 

Now for the L97P1 use this variable right out of mplmaster:

fmt P 5 nspring$ #Number of spring cuts

 

Put it on a line by itself at the bottom in the threading cycle you use like so:

 

pbld, n$, "L97", *nspring$, e$

 

HTH

 

[ 04-02-2008, 12:30 PM: Message edited by: Crazy^Millman ]

[crazy^millman]

Was this of any help to you???

[bigjohn]

It certainly was for me Ron. I'm trying to modify a post for an Index turming centre with C Axis twin turret, twin spindle and Sinumerik control.

 

Aren’t I lucky to have read this post?

 

Thanks Ron.

 

 

John

[nofalloff]

Yes,very much so. Thanks Ron, I think I understand. I've been home with the flu since I posted my question but I hope to be back at work tomorrow.

[crazy^millman]

Ok hope you get well soon, and if you have any questions or get stuck just post them up and we will see if we can help you out.

[Post dept]

nofalloff,

 

You really just have to get into the pg76new post block, rip it apart, and put it back together again.

 

You'll get it!

 

Brett

[nofalloff]

The feed rate is giving me a bit of trouble. I need it to be out put as thread pitch in the form of R20=.07692 (for .5-13 thread). In the questions there is the option to output feed character as either F or E. this is under the General out put section:

 

thread_address : 1 #Thread pitch address for lathe threading, 0 = Use F, 1 = Use E

 

In the pg76new block the second line outputs the feed by calling pffr block which I believe is where the feed is derived. is this correct?

 

How do I force it to out put the feed with a Charecter other than E or F?

 

thanks

 

peter-

[nofalloff]

Got it! After figuring out the logic for the F or E output from after the thread_address I just changed the appropriate string declaration from:

stre "E"

 

to

 

stre "R20="

 

quote:

---

You really just have to get into the pg76new post block, rip it apart, and put it back together again.

 

You'll get it!

 

Brett

---

Brett, It's turning out to be quite a bit more than tearing apart pg76new and changing a few format statements. but I'm making progress. I have a couple more questions but I'll post them in new threads once I have a better idea what to ask and have put more time into trying to figure them out my self.

 

 

peter-

[Guest CNC Apps Guy 1]

Brett Thomas, how the heck are you man??? LOng time since you've crawled out of your cave eh???

 

SHoot, that just reminded me, I owe you a CD... DAMN!!! I'll get it out tomorrow morning.