NEED HELP WITH CODE WIZARD

[modulus]

I am trying to configure a post proc for our Mori Seiki DL20MC
I'm stuck at the moment with outputting the correct tool change code

Our lathes all change tools this way:

G00 TO1O1;

My posts always output

T01 G43 H01

If I use one of the old templates the output is fine but then I can't get the C Axis working.

The code constructors look the same in the old style and new, so I guess something is configured wrongly elsewhere.

Anyone know where I'm going wrong?

Andy

[jsanders]

Hi Andy,
Turn on the 'Generate Code Constructor Trace' on the NC Debug page of the NC Style section in Code Wizard. Then compile the post. This adds a helpful debugging line in the posted code, where prior to the code is the code constructor that caused the output.

Your reseller should be able to assist you with developing a turn key post for your company's CNC machines. While the Code Wizard does make it possible to edit posts without syntax knowledge, there are many tricks that someone experienced with both proper Edgecam usage and post development can use to quickly configure a post that gives you the edit-free CNC code that you're after. Plus, the Code Wizard will allow you to maintain the post, add new functionality, build new posts, etc.

Hope that points you in the right direction.

Joe

[modulus]

Thanks Joe, actually I turned on trace after reading other posts here. Doesn't give me any help though in this instance. I think I'll just wait for the training, could spend a lifetime trying to figure this out!

Andy

[scudzuki]

Looks like you have 2 issues, number one, the wrong letters in the format table, and number 2, the wrong syntax (wording) in the cycle definition.

Can you provide a few more lines from each program, including several preceeding and several following the lines you included?

To verify, the toolchange line is G, double zero, space, T, capital O (not zero), turret number, capital O (not zero), register number?

If I understand correctly, the control on the Mori does not need an M code to specify a toolchange? In other words, the line
G00 TO1O1
means change tool, tool 1, assume length (or both) offset(s) from register 1?

If you PM me your email address, I can send you a document that might help a little.

Joe

[reedye]

To get the output you want. In code wiz go to code constructor and expand(click on the plus) then look for either Turret Toolchange or ATC Toolchange depending on wheter your machine has a turret or a tool changer. Expand and you will find Core Toolchange. open this selection and you will see the codes to create a tool change seqance. There shoud be a line tha looks like
[DELETE][BLKNUM][TURRETNO][TCHANGE][LENGTHOFFSET] remove [TCHANGE] then place you cusser before [TURRETNO] then under Valid Tokens double click on RAPIDGCODE. Your line should look like this [DELETE][BLKNUM][RAPIDGCODE][TURRETNO][LENGTHOFFSET] Next click ok on the bottom of the window. Now got back up to the Format Table. This will open a window that has word formats. move down the list under Letter Description untill you find Tool length Offset and highlight it. under Letter Address you should see H there is a space in front of it. Remove both by backspaceing.
click OK at the bottom of the window. Hit the recomplie buttion and you shou get the output you want. These Token names are for a Mori mill-turn so yours should be the same or very close. PM me with an e-mall address if you need more help

Ernie