NewB here need Post info

[AETOOLS]

First time user. Looked and searched the forum, found a lot of helpfull info however, there are several things I want to do to tweak my posts, I would like to have line numbers post only at tool change or process change. I don't want to ask to many questions all at once so I will stop there. Thanks.

P.S. great place for us MasterCam users

[Jimmy Wakeford from Barefoot CNC]

Find:

omitseq : no

and change to:

omitseq : yes

 

this will set post to NOT output sequence no's

 

then everywhere you want a seqno:

 

omitseq = no #add before line

n, *t, "M6", e

omitseq = yes #add after line

 

not the slickest way, but works

hth

[Charlie Pierson]

conversely, you could strip the n, from all of the output lines that you don't want sequence #'s and leave omitseq = no

 

cp

 

ps: welcome to the forum

[AETOOLS]

Thanks Jimmy, I will have to give that a try. Charlie thanks for the input but I am trying to avoid that. I am trying to get all of our posts edit free so when I have out tool library and material library set I will be able to make different operation libraries so other programmers here can program any machine and still have the same consistency. U2 have any other nice options that can be added to post or a way to save the operation and tool sheet without loosing the header in a Doc format? Thanks

[Mike Mattera - TFM]

Hi Joe,

 

welcome to the forum.

 

Set "omitseq" to 1 or yes. Then find the psof section and deceide where you want the block number to appear. Insert this line. Now do the same for the ptoolchg section of the post. If your running one of my Mill post MPFANUCV9_3X you find an example of this.

 

Actually if your running one of my posts, all you have to do is set "omitseq" to yes and it will already do it.

 

pbld, *n, e

 

This will force (*) the n number.

 

Mike Mattera

[NOTW Programmer]

I have omitseq = -1 #To enable for LCC

and in my machine definition I have #Output sequence #s off but I set Start@100 and Inc of 1 for LCC

 

Here is the Code I have in order to get an N + 1 at the G28 every toolchange.

code:

---

# Toolchange / NC output Variable Formats

....

#------------------------------------------------

fmt N 4 seq_tool_n #Sequence Toolchange <--- Insert this variable

fmt N 4 n$ #Sequence number

......

ltlchg$ #Toolchange, lathe <--- search for ltlchg$

#Toolchange g50 position

seq_tool_n = seq_tool_n + 1 # Sequence numbering - Just for ToolChange <--- Insert this to use variable

pbld, n$, seq_tool_n, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$ <---Insert seq_tool_n before *sg28ref (G28)

---

Voila, Im still working on getting my G70 to pick up the right P and Q; as of now it picks up the op1's P and Q for every finish OP. Can anyone help ?

[Colin Gilchrist]

Is your post based on MPMaster? It should be:

 

code:

---

tseqno      : 0     #Output sequence number at toolchanges when omitseq = yes

#0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number

---

This switch is ued to enable sequence numbers at toolchange.

 

You have two options:

 

1= Sequence number indicates toolchange number

 

2= Sequence numbers match the tool number.

 

Both are useful.

 

HTH,