Author Topic: Okuma E100, G28 & friends  (Read 1631 times)

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Okuma E100, G28 & friends
« on: April 04, 2012, 06:54:12 PM »
I need to make some edits to the Generic Okuma post & haven't found what I need yet in the forums.  Can someone, please, point me in the right direction on the following?:

1) How do I get the G28 stuff to go away in the Generic Okuma post?  The Okuma E100 control we have does not support such a g-code. I tried to "comment out" the writeBlock lines in the onSection & onClose function if-statements where they occur.  That didn't work.  Don't laugh too hard! Rookie attempt! :)

2)An "O" is added to the file name at the top of the program.  This causes an alarm.  The file name needs to be enclosed with parentheses on an E100 control.  I'm pretty sure it's the same for the P200, too.

3)The tool number appears in parentheses at the END of the Operation.  I would assume that logically would be at the beginning of the tool.

4)I would also assume the Operation Comment would follow the M01 from the previous Operation.

5)How do I add a Block Delete "/" before the coolant-on command and the next tool preload?  Kinda handy for proving out program.

Thanks,

Shane

René Fonseca

  • Development
  • Administrator
  • Hero Member
  • *****
  • Posts: 1928
Re: Okuma E100, G28 & friends
« Reply #1 on: April 05, 2012, 12:30:13 PM »
1. Does your control support something like "G16 H0 G0 Z0" instead? You can disable any output by commenting it out using either the "/* COMMENT */" or "// COMMENT" comment style syntax. I didn't update the post for this.

2. Look for "writeComment(programName)" in the attached post.

3. I'm not sure what you mean. I do not see any such output.

4. The post has been set up to write the operation comment right after any required machine retract. Can easily be moved to the desired location. The optional stop M1 is only output on tool changes and you wont have a tool change if 2 operations use the same tool.

5. Look for "writeOptionalBlock" in the attached post.

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Re: Okuma E100, G28 & friends
« Reply #2 on: April 05, 2012, 08:59:57 PM »
Rene,

Thanks for your help.

1) G16 is described as "Selection of work coordinate system (one-shot)". This is in contrast to G15, which is modal and is what your Okuma post correctly uses.  I don't know what G28 or G16 do on other controls, but the programs work perfectly simply deleting those lines.  Trying to comment out the lines gives me errors associated with funtions 'onSection' and 'onClose'...unsupported command 11.  See note below.

2) Great!

3) Sorry.  I got lost in the woods.  This is what had me confused: the first operation's tool number doesn't appear at the beginning of the operation like all of the others do.

4) That's fine...just gotta get used to it.

5) Thanks.  I don't need for the M9, so do I delete/comment out these lines?
case COMMAND_COOLANT_OFF:
    writeOptionalBlock(mFormat.format(9));
    return;

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Re: Okuma E100, G28 & friends
« Reply #3 on: April 05, 2012, 09:16:17 PM »
1&5) Correction...trying to comment out the Coolant Off "writeOptionalBlock" causes the errors.  How to I remove the block delete from the coolant off command.  Only needed for coolant on and pre-staged tool.

Thanks,

Shane

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Re: Okuma E100, G28 & friends
« Reply #4 on: April 05, 2012, 09:39:44 PM »
Fixed G28/G16 and block delete on M9.  Think I'm getting the hang of this.  JavaScript reminds me of Pascal, though I'm going back a couple of decades worth of cobwebs!  :)

Thanks for your patience!

Shane

PS  Attached is what I have so far.  I'm going to work on getting the comment line right after the tool line so they're together.  I also only want a line/sequence number at the beginning of each operation that is essentially the tool number.  N18 for Tool 18, N11 for Tool 11, etc.  Makes it easier for restart and fits what we're currently doing with MasterCam.

René Fonseca

  • Development
  • Administrator
  • Hero Member
  • *****
  • Posts: 1928
Re: Okuma E100, G28 & friends
« Reply #5 on: April 05, 2012, 09:40:36 PM »
Try this one.

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Re: Okuma E100, G28 & friends
« Reply #6 on: April 05, 2012, 10:39:23 PM »
Thanks again.  Looks like I'm almost there.  Trying to get the visual & functionality similar to what our operators are already used to.  If not, well you can imagine! :)

In the attached .min file, I've manually entered sample text for a second operation with the same tool.  Having a hard time figuring out what & where to put in the post.  Can you point me in the right direction again, please?

Unless I've missed something, the version of the post in the zip file is working well.  Also, edited max spindle speed and max tool #, etc.

Shane

René Fonseca

  • Development
  • Administrator
  • Hero Member
  • *****
  • Posts: 1928
Re: Okuma E100, G28 & friends
« Reply #7 on: April 07, 2012, 07:28:58 PM »
Here is my updated post. Since the same tool can be used multiple times in a program I use the operation id instead of the tool number for the block number.

I also cleaned up the post.

Shane Vest

  • HSMXpress User
  • Jr. Member
  • *
  • Posts: 13
Re: Okuma E100, G28 & friends
« Reply #8 on: April 09, 2012, 03:59:39 PM »
Rene,

You've been great in responding to our post needs!  You're making a strong case against my Mastercam VAR's tech support.

Thanks for cleaning up the post some more.  Just a little bit about why we'd like the block numbers to be the same as the tool number.  The e100 and p200 controls allow the operator to restart a given tool at the second, third, etc. "instance".  As an example, if the operator needs to restart tool 12 at the point the tool is used for the third time, he can perform a Restart for tool 12 at "N12 instance 3".  The control goes thru the program and is ready at the 3rd N12 it gets to.  Otherwise the operator needs to go thru the program and find out which block number happens to be at that location.  Mentally, without having to look at the program, he already knows which tool number he needs and which instance he needs to restart at.


René Fonseca

  • Development
  • Administrator
  • Hero Member
  • *****
  • Posts: 1928
Re: Okuma E100, G28 & friends
« Reply #9 on: April 09, 2012, 04:35:05 PM »
Glad to help.

I understand about the block numbers. I think this multi-instance feature is not supported on many control.