Okuma OSP5000 post questions

[Dan S.]

Hi all,

 

 

I am new to mastercam and I am trying to edit a post used to program an Okuma MCVA with an OSP5000 control. I have several questions.

 

I need to output a M52 on the last position line of all canned cycles. I can get it on its own line after the last position (before G80), but it needs to be on the position line.

 

The operators are asking for a "N" number at every tool change starting with N100. They do not want it to be the same as the tool number. They wan't it to change by 100 (N100,N200,ect) at every tool change even if the tool is being used a 2nd time. I'm not too sure how to do this. I can get a "N" number the same as the tool number, but that is as close as I have come. It isn't all that great, because if you use say tool #1 a second time you get N1 again.

 

The last thing I have to fix is that the work coordinate output is starting with H00, not H01. That may be inside mastercam as a parameter setting, I'm not sure. Like I said I'm new to mastercam.

 

Any help would be appreciated.

 

 

Thanks,

Dan

[Roger Martin from CNC Software]

Dan,

 

What PST is you Okuma post based on?

The MPOKUMA.PST that is on the v9 CD?

 

All your requests a fairly straight forward, but without knowing the current state of your PST it's a bit of a guess as to where to point you. (Unless you're familiar with doing Post changes).

 

Top of the MPOKUMA.PST -->

code:

---

# Post Name           : MPOKUMA

# Product : MILL

# Machine Name : GENERIC OKUMA

# Control Name : GENERIC OSP5000M, OSP7000M & U100M

# Description : GENERIC OKUMA MILL POST

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Executable : MP 9.13

---

[jimspac]

Most of the things you ask about like H0 to H01 I do in the editor( Cimco). I had modified the post to not pre stage tools as my 1985 Okuma 5VA would lock up. The post as supplied with Mastercam was very compatible for 3D and only pre staged in 2D. We have the OSP5000M on 2 machines and they are my favorites within a sea of Haas VFs.

[Mick]

If you want a dialed in post for the OSP series of controllers, talk to your reseller, and get them to ask Inhouse Solutions for the MPMaster Okuma Post Processor. That post pretty much works right out of the box. I can vouch for it, because I use it on a number of Okuma Vertical machines.

 

Jimspac, there must be something wrong either with the format of the code, or the machine itself, if the MC5VA locks up when prestaging tools. I used to programme a MC5VA with an OSP5000M-G control, and prestaging work great with it.

 

I agree, they're great controls. Out of all the machines I've programmed, I much preferred the OSP's . For me, the jury is still out on the E100M control. The "window" type control is a bit hard to get used to

[jimspac]

Mick,

I believe that the issue with pre staging is the vintage of the control on that machine. I am sure that the same control on our 4VA(1989)does pre stage. I do not prog that one myself so I can only guess.

[md]

Check your mail

 

 

I'd rather die on my feet than live my life on my KNEES

[Dan S.]

Sorry for the delay in responding, I was out of town for a few days. The post I had to start with starts like this:

 

# Post Name : MPOSP

# Product : MILL

# Machine Name : OKUMA MILL

# Control Name : OKUMA OSP5020M

# Description : OKUMA MILL

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Executable : MP 9.13

 

I am not really looking for someone to modify or tweak a post for me. I would rather learn the language myself (at least to some extent).

 

I am not afraid of some hand program editing either, but would for obvious reasons I would like to have to do as little as possible.

 

I have made several change to this post already. Mostly just trial and error. It seems to work so far, but I'm sure there are mistakes and it may not work in all situations.

 

Dan

[jimspac]

I found the MPOKUMA post off the CD was closest match for the OSP5000M-G controls we have, the MPOSP didn't come as close.

[Roger Martin from CNC Software]

Dan,

 

Output ‘M52’ on the final X,Y position of a canned cycle.

Not difficult (easy for me to say, eh?), but something that would definatly trip up most.

First, we need to have a way to know we are processing the final position move of a drill cycle. We need to “look ahead”. To do that I activated the ‘getnextop’ and then added a call to a new postblock that check to see if the next action is going to be the ‘G80’ and is so output the ‘M52’.

 

The MPOSP post already had (some) special ‘N’ numbering logic (N =T#)

Just added a variable to use as a toolchange counter and altered the existing formula to use it.

 

The 'H??' offset value is set using the ‘Work offset’ setting on the T/C plane page of the toolpath parameters. What I did in the MPOSP is add a logic test (like was already in the MPOKUMA.PST) that checks for the situation of the ‘workofs=0’ and forces it up to be ‘1’.

 

You can see all these changes by downloading the MPOSP.PST from the forum FTP site

It is in the ‘Text_&_post_files_&_misc’ folder.

*The changes are marked rm (which is enclosed in the angled brackets that would not appear on this posting)

[Roger Martin from CNC Software]

quote:

---

I found the MPOKUMA post off the CD was closest match for the OSP5000M-G controls we have, the MPOSP didn't come as close.

---

And if you find this to be true for you...

I've already made all the changes to the MPOKUMA.PST last week.

 

*The 'H00' change was not needed, because the MPOKUMA already had that logic.

*The special line numbering took a little bit more work, because the MPOKUMA.PST had no special 'N' numbering logic to start with.

*The 'M52' output logic was the same.

[Dan S.]

Thanks all. I now have a working post. The code looks great....just what we wanted.

 

Thanks again

 

 

Dan