Post editing issue.

[cjdavis618]

I have both version 23 and Version 24 and I am trying to find the Post editor that I have seen mentioned that allows editing of the posts for variables etc. I have found the "Machine editor" but that just lets me set machine options.

I have tried to manually edit the post I need to take the remarks out, but it doesn't seem to change anyting on the posted gcode once I do that. I have spent a few hours on this and can't seem to make any progress with it.

Where do I get this "Post editor"

Thanks
Chris

[BurrMan]

The MillEditPost.exe should be in the root of the V23 installation... But it is not recommended for V24.. Your best bet, since you already started out this way, is to use a text editer like Notepad.

We should just figure out why your edits arent posting the changes you made..

Be sure that the post you are editing is the actual one you are posting with. To do this, make your edits and csave them with notepad, then when in your BobCad file, right click the selected post and choose edit, then navigate to and choose the one you just edited and post. Note: BobCad will retain the selected post within it's file and post with that, or the default the first time through.. In other words, if I have a post named "Burr" and you open my file and just select post code, it will post with a default post because there is no Burr post in your folder) So reselecting after editing may be nessasary.

With some of the newer OS's and UAC enabled, you cant save a post you are editing to the BobCad post folder with notepad. You will have to save it to somewhere else, then copy it back into the post folder to overwrite what is there..(The only way around this is to start notepad first, as Administrator, then open and edit the post... You can create a shortcut that will launch notepad with admin rights for this)

The Variables selection comes from a text file called "PostVariables.txt" in the posts folder. You can just open this file to read the variables and desciption to use in your editing..

If you really want the editer as a learning tool, you can find it here:

MillEditPost

[cjdavis618]

Burrman, Thanks for responding.

I just got version 24 today for the improvements on the milling of profiles and nesting features. But I have looked all over the Bobcad software folders for any .exe file and never could find anything but the machine editors... There is no file by that name on my system at all. I have searched the entire drive. And the CDs for it.

The short of it is this. My SX3 mill is set with Mach 3 to move to a position for a tool change and wait for me to insert, then start again. Obviously, I am using offsets and quick change tooling, but do not really have an ATC. (I'm the ATC.. lol)

I have both post files for Mach 3, one is with ATC and one without.

When I use the one without, everything is pefect except my tool changes and offsets are remarked out. When I use the ATC version, there is a G53 0 command that sends my mill into the limit switch because mach 3 isn't clearing the tool offset and is ignoring machine zero. (Mach has decided that limit switches are ignored when offsets are applied during tool changes, or at least that is what I understood from them.)

I just need to edit one or the other so I can either have my tools un-remarked or the G53 gone.

Like I mentioned, I have copied my original post out to a backup file, then renamed the one I was testing with and I have seen what lines I should edit, but it doesn't change anything when I remove the offending characters and save the file. I did verify that the changes were in the file, but when I post an operation, the lines are still remarked out.

For example,

The no ATC version says this:
n,inch_mode,"G40","G49",work_coord,cancel_drill_cycle,absolute_coord,"G91.1"
n,"G53","Z0."
" "
system_comment
feature_name_comment
" "
n_forced,";",t
n,s,spindle_on

ATC version says this:
n,inch_mode,"G40","G49",work_coord,cancel_drill_cycle,absolute_coord,"G91.1"
n,"G53","Z0."
" "
system_comment
feature_name_comment
" "
n_forced,t,"M06"
n,s,spindle_on

When I take a section from the ATC and insert it over the No atc file and save it, no changes happen with the posts. I did verify that the file name was the right one and selected in the mill post settings. What is strange to me is that both posts show the n,"G53","Z0" line but the no atc version has them remarked out when I post with it and I can't seem to find out why. They are the same on that particular line.

I thought maybe that I had to have the editor to make the changes since nothing else seemed to work for me.

I'll try again tomorrow and make sure I wasn't missing something. Thanks for your help.

[Perfect Circle]

Here ya go
Good Luck~!

[BurrMan]

cjdavis,
Remember the post files are just simple text files, so if you are changing something and it's not reflecting in the posted code, you will want to double check that you are editing the post that you are posting with.

Good luck.

[Sowen]

Below is a link to a video that covers how to modify a post processor.

[cjdavis618]

Thanks guys, I appreciate the help and will try this as soon as I can get time to go back to the shop.

I will follow up after that with the results.

[cjdavis618]

I finally got back around to editing the posts again tonight and here is what I found. I was looking at the individual lines instead of the block of commands.

I found a program called winmerge that allows you to open and compare text files and it will highlight lines that are different between the files.

I was saving the files fine, but what I didn't change was the "Start_add_block_delete" and "stop_add_block_delete" above and below the line that I wanted to have active. Once I erased those from the no-atc test post I made, all was well.

Thanks for the info on this. I appreciate the support.

[BurrMan]

Thats good. Pradator will do simple compares on files also...