small posting problem

[cherokeechief79]

since weve loaded x9 if I pick a drill from the catalog its not posting its description..for instance if I pick a no 7 drill all it outputs in the code at the top of the prog is (T3   I  NO                                                  I  H3    I   D3    D0.201         I   DRILL/CBORE)

 

and at the actual toolcal in the prog this is what I get      T3 M06  (NO)

 

any ideas?

seems to be only with drills

 

 

[cherokeechief79]

any ideas on this?

its drivin me crazy today.

[jlw™]

Did you upgrade the tool db to x9 or are you picking from generic X9 db?

[cherokeechief79]

didn't upgrade as far as I know.

how do I do this?

thanks for the reply.

[jlw™]

Use migration wizard under "File" menu. I had to update my tool db's to get it right but I had custom geo for many tools.

[cherokeechief79]

ok ive been playing around with this and found something out.

if I select a drill that is a fraction(1/8 or so) it will output (1/8 drill) in the description at the top of the program and also when it calls the tool. just like it always has for me thru many many years.

if I select a drill that is a number drill,it will only output (NO) even though the tool name is say"NO. 77 DRILL"

any ideas?

this is driving me batty

[Guest]

For sh!ts and giggles try changing the drill  name to 

 

NO_77 Drill

 

Get rid of the period

[cherokeechief79]

thanks john!   that did work.

 im just selecting tools from the standard tooltabe included in mc.

is ther something in my post not letting it read past the period?

[Guest]

thanks john!   that did work.

 im just selecting tools from the standard tooltabe included in mc.

is ther something in my post not letting it read past the period?

 

I don't think it's the post, I have seen this exact issue in Active reports as well....I believe it has something to do with how a . is being handled somewhere in the software

[Colin Gilchrist]

To find out, try just posting the NCI file. That will show if the string is present for the Tool Description, or if this is a bug inside Mastercam, where maybe the software is truncating the string prior to writing it to the NCI file...

[crazy^millman]

Colin please correct me if I am wrong. MP.dll does some strange things no way or really knowing looking at NCI when using MP posts. Now if you are using a 3rd Party like ICAM or something like that that only uses the NCI to generate code then someone see what is going on? I remember back in the V7 to V9 days where many outside companies were creating their own MP.dll for their posts because of all the things MP.dll does that most people never see or are aware of. Has that process changed and NCI to PST does all the work and the MP.dll has no bearing on the outputted NC code?

[Colin Gilchrist]

Hi Ron,

 

Yes, MP.DLL does some things "behind the scenes", which is why I suggested testing the output of the NCI file. The PST file consumes NCI data, and outputs formatted NC code. That said, MP.DLL is also kind of "consulted" when writing the NCI data. To some extent, I also believe it influences the creation of the NCI file. I'm not sure what happens if you assign another "Post DLL" in the System configuration. My suspicion is that the NCI is then just generated with some "default" MP values. Maybe the same "Command Variables" are still at play? I'm not sure.

 

I know for example that the "Max characters in NC Comment" setting in the Control Definition file will set the max String length for string parameters that get written to the NCI file. So if you put in "80" characters, MP will truncate your strings prior to them being written to the NCI file.

 

My guess is that there is some provision for using the "Dot" (.) operator, that has changed the way MP.DLL is handling the strings internally. I'm just guessing, but I suspect that the strings are being truncated by MP, prior to writing them to the NCI file. If that is the case, then this is a Mastercam Bug, that would need to be fixed by Mastercam.

 

However, it is also possible that the string is being written to the NCI file correctly, and the truncation is happening during output. If that is the case, then it might be possible to read the same string from a different source, to avoid the truncation behavior.

 

My guess is that MP.DLL has been enhanced in some meaningful way, but there was an unintended consequence...

[cherokeechief79]

it posted properly to the nci file.

it had the complete description including the period.

does this mean its the post?

[cherokeechief79]

what if I went into the tool library and deleted all of the periods after the NO on each tool?

[cherokeechief79]

ok found something else.

I looked back at some old programs I wrote and number drills were described as   "#7 drill" not NO.7

 

this must be the difference.

I don't really have any custom tools so is there a way I can change their description in the mc library tu use the # sign?

[cherokeechief79]

ok so I really messed things up now.

I opened the inch lib that my post was looking at and did a replace all NO. with #         it did over 700 instances.

now nothing at all will open in that library but when I switch to BIG IN MM library all the tools are there and the drills also have the # sign ahead of them like it should.

it must have changed something somehow.

[jlw™]

To find out, try just posting the NCI file. That will show if the string is present for the Tool Description, or if this is a bug inside Mastercam, where maybe the software is truncating the string prior to writing it to the NCI file...

How do you post the raw NCI file?

[Mick]

How do you post the raw NCI file?

 

In the posting dialog, check the NCI File checkbox, just like you would for the NC file.

 

By checking Edit, it will open up in the default editor.

[jlw™]

Thank you! I feel like DUH! How many times have I looked at that? I always just green check it. In fact it gets on my nerves having a dialogue. I miss just hitting F9 to post.

[cherokeechief79]

looks like the "big inch library " included in mc has number drills starting with NO. and "bigMMinch lib"drills start with #.

this lib works for me.

I always thought this lib had metric tooling in it too but it looks like there are just metric engraving tools.

 

how do I direct my config to look for this tool lib instead of the other?

when I tyr to change operation defaults it is grayed out where I would set the tool lib.

[CJep]

how do I direct my config to look for this tool lib instead of the other?

when I tyr to change operation defaults it is grayed out where I would set the tool lib.

That's a setting in the machine definition file.

Go to settings, open the machine def, and in the row of icons at the top go to general machine parameters. (to the left of the control def icon)

In the gen machine params there is a tab for setting the default tool library.

[cherokeechief79]

oh well that didn't work

this has proved to be quite a problem for me.

if I select a tool from the "big MM INCH " catalog it does have all inch size tooling in it but it uses metric values for the diam and length.

back to the drawing board I guess.

i think i need to get my post to stop terminating anything beyond the period in the description.

[Colin Gilchrist]

Have you, by any chance, added any code to the post to change the way comments are handled?

 

Try searching your post for 'smatch'. Do you have this variable initialized? Do you have a 'pcomment_out' post block?

 

The reason I ask is that I added some code for "multi-line" output that will break comment strings into multiple, individual, strings, based on a "matching character". That "match" character gets stripped from the lines during output. Do you happen to have "smatch" set to "."?

[cherokeechief79]

got it finally!

thanks for all of your input.

one of the knowledgeable guys from engineering came down and made a small change in my post. now it reads beyond the period.

I reloaded the "big inch library " and all seems to bo ok.