operations won't stay checked

[buck30]

I check all my operations i wont to post and somhow thye become Unchecked. Well one of them stays checked.

I seem to have this problem before but for the life of me I can't remmebr how to correct this.

 

Please help me out here.

 

Still using X5

[TK-32™]

is the NC file the same for all ops?

do you have ghost ops?

[LaszloK]

I have seen that happen when posting but all operations ended up posted anyway. All are checked again once the posting operation finishes so I just ignore the fact that it only shows the one check mark. The real key to determine if you will get them all is the warning that pops up when all are not selected.

[buck30]

got it. I chaged the NC name and that fixed it.

This has happened to me before a few years back.

Thanks for your input and merry christmas out there in MC land.

 

and No Laszlok the remaining operations that became unchecked definetly did not post.

got it now so off to the next problem.

[PLANET]

Try selecting all the operations, hold your cursor over the toolpath group, right click, select "Edit selected operations", select "Change NC file name", when that box pops up just hit the green checkmark.

 

I get that sometimes when I go back & add an operation to a toolpath group that I have already posted.

 

Usually when it does it, it will post but not all together.

[buck30]

interesting you mentione that adding a toolpath Planet.

This is exactly what i did. got it now though..

[Christian Raebild]

You seem to have solved the problem, but I can explain what happened, as I have seen it a number of times at customers too.

 

What happens is that some of your operations are getting different NC names and/or paths, so they are not post processed together.

 

It usually happens when adding operations to a file that has been edited on another PC or if the NC file path has been edited in the configuration, so the new operation(s) get the NC file path of the new PC or new configuration.

 

It might also happen if Mastercam's configuration is set to give the NC file the same name as the MCX file, if you have saved the MCX file with a new name, perhaps to save the old version while trying to improve on the toolpaths.

 

The solution is as has been pointed out to select all operations and then right click and choose "Edit selected operations" and the "Change NC file name", and then click OK (you don't have to actually change the NC file name that is listed).

 

I just thought you might like to know why that problem happens.

[uncle_dolan]

I have seen that happen when posting but all operations ended up posted anyway. All are checked again once the posting operation finishes so I just ignore the fact that it only shows the one check mark. The real key to determine if you will get them all is the warning that pops up when all are not selected.

 

This can be dangerous ground! If you are experiencing the same problem (different .nc names), what happens when you select all and POST them, is that it wil post all files under nc filename "a", and then post all files under nc filename "b". So you end up with either 2 programs, or you overwrite ine program with the other if manually prompted for filename on POSTING. You can see this will be dangerous if say your roughing and finishing do not post in the same file...dont really want to finish without roughing first...Just a note of caution! ALWAYS CHECK YOUR CODE!

[Bruce Kanzelmeyer]

I have noticed that if you modify the default suggested name for the nc file when creating the first operation ( when mastercam asks you to confirm it's suggested name), that as you add operations, MCX will just insert the default nc filename without giving you the option of modifying again. In other words, your new filename is NOT automatically remembered and carried on through the remaining operations in that toolpath group.

[Christian Raebild]

Uncle_dolan: I don't think this problem can get the finshing operations to overwrite the roughing operations, as the operations would get written to different files, but yes, you should always check your code. If you expect both the roughing and fihishing operations to be written to the same file, then you might end up only sending the finishing opertaions to the machine if you aren't careful. It won't get two programs which both contain all operations, though, each of the posted programs will contain different operations, as each of the operations will onlt be posted to one of the files.

 

Bruce Kanzelmeyer: That depends on your Mastercam configuration. If you go to the "Toolpath manager" page and look under "NC file", then you can select "Prompt", "1st operation only" and "Last operation's NC file". That will go a long way towards ensuring that all operations have the same file name and path, so all operations get post processed to the same file. As far as I remember the only way to get operations post processed to different files with that setting (other than intentionally setting different files) is if you continue work on a MCX file where the original NC file path doesn't exist on the PC you are continuing work on.