[wiley125]

Fadal VMC 88HS control verson 1

[ObrienDave]

Which Fadal do you have?
I can help you with modifying the generic Fadal post that comes with MasterCam.

[wiley125]

I have a Fadal 4020 vmc 88hs verson 1
i am having trouble with work offsets i do not want to use any E or the G92 codes, and also when i program a drill cycle the first hole location is before the canned cycle so the first hole gets it skipped. As I look through the nc file everything else looks fine.

[ObrienDave]

Ok, let's solve one problem at a time.

For some reason, I get an error at line 547, if mi1 <= one, #Work coordinate system.
As far as I know, there is nothing wrong with this line.
Let's try it this way...
Make a ZIP file from both the .pst and the .txt files and repost the zip file to this thread.

The G92 is easy to remove but, why do you NOT want to use E fixture offsets?
If I remember correctly, Fadal supports G54-G59 as E1-6.

If you like, you can delete the text of your post from your previous message,

[wiley125]

I dont want to use the fixture offsets because we work on big parts, never small so we dont use them, we just zero the machine over the part, and leave Z at the tool change height. It wouldnt be a big deal if i could just set the fixture offset to zero. But I couldnt find it. But here is the zip file Thanks

[ObrienDave]

Ok, that solved the error problem, thanks.

Here is a little drill program I posted using your post file.
I really don't see anything wrong with the code.
It is posting E0 (fixture offsets off) and no G92 because I turned Misc. values off.
Please see attached image.

If you can, please zip a MC8 file or post a bit of the code you are having trouble with.

[wiley125]

Yeah its doing the samething with the drill cycle.

Its posting this
N5 G0 G90 S1069 M3 X4. Y1. (Positioning for 1st hole here)
N6 H1 Z2. M8
N7 G81 G98 Z-.5 R0.1 F4.28

it should post this
N5 G0 G90 S1069 M3
N6 H1 Z2. M8
N7 G81 G98 Z-.5 R0.1 F4.28 X4. Y1. (Positioning for 1st hole here)

[ObrienDave]

I fixed the post to do it that way.
I left the original 1st hole positioning code intact because I feel it is safer.

It now posts:
N4 T1 M6
N5 G0 G90 S1069 M3 X4. Y1.(1st hole position here)
N6 H1 Z2. M8
N7 G81 G98 X4. Y1. Z-.5 R0.1 F4.28 (and here)

It's easy enough to remove if you don't want the first hole code there.
I commented the changes I made to the drilling sections.

[wiley125]

Thanks, what did you change and where? Is that the only thing that was changed? And thanks for the help. How does the fadal format 1 and 2make the machine act different?.

[wiley125]

I send the program to the machine and the program number and name does now show up. It is in the nc file and looks correct, but it doesnt show up on the fadal. I was having trouble sending it to the machine through mastercam so i used another program called dostek dnc file manager. And it worked fine. Is the problem the file manager or the fadal. How do I find out?

Here is my program just to be sure that it looks correct.

[ObrienDave]

Ok, I'll answer one question at a time.

Thanks, what did you change and where?

A1.
What I changed is commented in the drilling section of the post.
Look for,

pdrill #Canned Drill Cycle - G81/G82
pdrlcommonb
pcan1, pbld, n, *sgdrill, *sgdrlref, pfxout, pfyout, pfzout, pcout, #changed pxout, pyout, to pfxout, pfyout
prdrlout, dwell, *feed, strcantext, e
pcom_movea

I had to change all of the start blocks for fixed cycles or none of the other cycles would have worked the same way.
Remember, anything after the '#' is considered a comment and ignored.

Is that the only thing that was changed?

A2.
Yes, in order to remove the G92 and force E0 all you have to do is turn off the Misc. integer button.
If you really want it done properly, I would need to edit the post to actually remove or ignore the codes.
However, if in the future, if you decide you need to use fixture offsets, re-implenting the various codes would take more work than it is probably worth.

How does the fadal format 1 and 2 make the machine act different?

A3.
There are quite a few differences between Fadal format 1 and 2
The 2 biggest are the macro programming langauge and how the machine moves at the beginning and end of the program, and tool changing.

For macro programming, format 2 is very close to the Fanuc macro language.
There are a few important differences that we don't need to point out at this time.
I can't find any examples to show you but suffice it to say if you got good at format 1 macros and ever needed to program a Fanuc you would be totally lost.

Format 1 machine behavior, for me, totally SUCKS!
For some reason, someone decided that the machine needs to move to the cold start position before the first line of code, after the last line of code and at every tool change.
To me, this is about the dumbest thing Fadal ever did.
Since there still is 4" of programmable +Z travel from the tool change position, if you ever needed to push the Z axis programming envelope with tall parts, or long tools, like I have had to do, I guarantee you will crash the tool, or part, or machine, or any combination thereof, using format 1.

If you like, I will PM you a copy of a Fadal post that I have personally used that takes advantage of the extra 4" of +Z travel.

I send the program to the machine and the program number and name does now show up. It is in the nc file and looks correct, but it doesnt show up on the fadal. I was having trouble sending it to the machine through mastercam so i used another program called dostek dnc file manager. And it worked fine. Is the problem the file manager or the fadal. How do I find out?

Here is my program just to be sure that it looks correct.

A4.
I forgot that Fadal does not like the program number to be zero.
Edit the NC file I posted to be Oxxxx, anything other than zero and it will show up in the directory.
Sorry about that.

Your program looks fine.

Good luck, have fun with it.
If I can be of further assistance please feel free to ask.

[wiley125]

Awsome thanks for all the help

[ObrienDave]

Not a problem.
You're welcome.

[wiley125]

I have tried using the program number without 0 and it still does not show up. Is there anything else the it could be.
It shows up in the nc file, but does not recieve that line, and only that line on the fadal.

[ObrienDave]

The O word must contain a number other than zero.
Avoid using numbers greater than 9000
Fadal uses some of those numbers for other fixed cycles like the embedded engraving cycle.
Fadal calls them 'fixed subroutines'.
Try making it O1234

Wait a sec, if I remember correctly, the O word will only show up in the program directory.
It will not show up in the program editor.
If the program shows up in the directory that is probably correct.
I might be wrong since it's been a few years since I used a Fadal.

By the way, you can download all of the available Fadal documentaton from:
http://www.compumachine.com/Support/DL-Fadal.htm

[wiley125]

Program directory? And the word shows up in the program editor. It still sends to the machine fine, but i wont be able to switch back to a program without losing the one loaded.

[David Russell]

I always use O7777 on every program it makes it alittle faster when bringing them in to the fadal