Post question

[gcode]

I'm using the MPLFAN post

When gear output code is enabled

(M40, 41, and 42)

the post puts the M41 and M03 on the same line.

The machine I'm programming won't accept 2 M codes on the same line.

How do you modify the post to output them on seperate lines.

I assume it has something to do with the variable

"prpm", but when I try to break it into 2 lines

I get a boolean error.

[Allan]

Depending on the era of your post the line would be in pgear postblock or ptlchg or ltlchg. Look for spdlon or something close as a string select near top of post (You will see the M3 there). Search further down in the post for spdlon and you will see where it comes out.

 

Can you post the prpm postblock?

 

Allan

[gcode]

I'm using the latest Fanuc lathe post.

Here's the prpm blocks.

When I try to put spindle_l and pgear

on seperate lines I get a boolean error

 

prpm #Output for start spindle

speed = speedrpm

if posttype = two, pbld, n, *sg97, *speed, *spindle_l, pgear, e

 

else, pbld, n, *sg97, *speed, *spindle_m, e

 

This is what prpm posts if css is active

G97S2728M03M42

 

[ 02-02-2002, 01:31 AM: Message edited by: gcode ]

[bryan.davis]

try this

 

quote:

---

prpm #Output for start spindle

speed = speedrpm

if posttype = two, pbld, n, *sg97, pgear, e

if posttype = two, *speed, *spindle_l, e

else, pbld, n, *sg97, *speed, *spindle_m, e

---

it should give you this

quote:

---

G97M42

S2728M03

---

it may not work but Ive not got my note with me today

[gcode]

bryan,

I tried a variation of your suggestion and it worked perfectly

 

This:

prpm #Output for start spindle

speed = speedrpm

if posttype = two, pbld, n, *sg97, *speed, pgear, e

if posttype = two, pbld, n, *spindle_l, e

else, pbld, n, *sg97, *speed, *spindle_m, e

 

Output this:

G97 S2523 M42

M03.

 

Its so simple when you know what you are doing.

Thanks very much, I'm embarrassed to say how long I fought with that

[Guest]

The Boolean error is caused by a syntax problem you need to format the statement as follows to avoid the problem and not have two "if" statements:

 

if posttype = two,

[

pbld, n, *sg97, *speed, *spindle_l, e

pbld, n, pgear, e

]

else, pbld, n, *sg97, *speed, *spindle_m, e

 

The brackets allow you to have multiple line of output, code, ect. in one "if" statement.

[Ryeker]

Please allow me to throw my 2 cents worth in here..! Whilst we are talking about "post" problems I have a question for you all. Using V8 If I am boring a hole on a lathe and the internal profile has reached the end, the post that I am using sends the tool to "G28 U0. W0." (no problem with that... it's just the timing that is the issue) as you may be able to visualize there is a Z+ move missing here to send the tool out of the part stock BEFORE the rapid move home. Does anybody have a clue what I need to add (and where) into the post to get a Z+ move....? As you can see below this could be a major crunch in the making...!

 

Here is the last few lines of code from a finish boring cycle:

 

G1 X.656

X.616 Z-1.0425

G0 X.5265

M9

G28 U0. W0.

T0800

M30

%

[Glenn Bouman]

Make sure that "Write home position clearance moves" is turned on in Job Setup. You also need to define your stock for this parameter to be available.

[Allan]

Make sure that you are using V8.1.1 this was an issue with Lathe V8.0

 

Allan

[Ryeker]

Thank you for the prompt reply's I will try them both...

[Ryeker]

OK so I know I have version 8.1 ( says so on the disk...! )... I download the 2 pathes that I need ( Mill & Lathe ) but when I double click them it gets 40% into the update and stops telling me that I have "Invalid Patch File C:mcam8m81-811rel.exe". What the heck is that about...? I have not used any accelerators to download the patch, they came in clean... so has anybody any ideas...????

[tm311]

I think this is telling you that theese patches

are not compatible w/ver 8.1,and you have to download the patch for 8.1.1 before they will work.

[Allan]

If you've changed your lathe8.txt file it will produce an error but not that one.

 

Check your exe date in Mastercam press alt-v it will display exe date.

 

Allan

 

[ 02-06-2002, 09:11 PM: Message edited by: Allan ]

[Ryeker]

I have had to repair my MasterCAM installation as it became corrupted whilst messing around with the update patches..! Jezz this is turning into a real pain....! I pressed alt-v and it tells me MASTERCAM version 8 (1.26.2001). The disc that I have is the 8.1 version. Am I using the right update patch..? Is there more than 1...? Your continued help is appreciated..!!!

[gcode]

Make sure you save the patch in the same directory

as Mastercam. Normaly this will C:/Mcam8 or Mcam81

 

Pay close attention to any error messages you get while running the patch. If you don't have Wire installed you'll get an error saying

"Wire.exe not found!" Just click OK and the patch will proceed.

[Ryeker]

OK I finally got the patches in... did a reinstall and redownloaded them into the mcam8 dir. It now says 8.1.1 when MasterCAM is running.. Thanks to all who helped..! However my problem with the boring cycle still exists. I have one further question for Glen Bouman, I could not find "Write home position clearance moves" in the Lathe job setup. What am I missing here Glen...? Also I have tried using the ref. points in the job setup ( I set the Z retract to 1.0 ) but it made no difference to the posted program. I was hoping that there would be a line I could input in my post processor to make ( force..? ) it to go to Z1. after a boring cycle. Thankx in advance.

[Ryeker]

OK I got it...!!! My post is now outputting what I want... Life is good again...!