help to edit mastercam post processor

[Moorej91]

I have got the boss 5 post processor from mastercam. The post does not work. I have 2 problems.

1. The post is outputting a metric path into a g70 inch. How do I change?

2. The post is outputting 4 decimal places. How do I change?

I have been into edit pst and changed the FS 2 to 0.4 0.3. Did not work.
changed it to .4 .3 still did not work, cahnged it to Fs2 2 0.4 0.3 as the book says and it gave an error message.

Can anyone advise me, I am new to editing posts

[Rekd]

Make a backup copy of your post if you haven't already.

Originally Posted by Moorej91 1. The post is outputting a metric path into a g70 inch. How do I change?

In Mastercam, go to Screen/Configure and select the Start/Exit tab. Select Mill9.cfg (English).

I think you're using Metric, this should fix it. A mod to the post may be needed if it's been chaned to process with the g70. Lets see what the first change does though.

2. The post is outputting 4 decimal places. How do I change? I have been into edit pst and changed the FS 2 to 0.4 0.3. Did not work. changed it to .4 .3 still did not work, cahnged it to Fs2 2 0.4 0.3 as the book says and it gave an error message. Can anyone advise me, I am new to editing posts

Put all your FS's back to what they were. You should never need to change these. If anything, create new ones.

In your post, find the FS that matches this one.

fs 11  0.3 0.3     #Decimal, absolute, 3 place

Then find

fmt  X  2   xabs        #X position output
fmt  Y  2   yabs        #Y position output
fmt  Z  2   zabs        #Z position output

and replace the "2" after the letter with the number, in my case above, "11".
FS 11 is for 3 place output. You may need to do other axis if you have more than X Y Z.

Note about editing posts, especially if you're new; only make one change at a time and check the output. Be aware of changes that affect things in other places in the program too.

[psychomill]

You're changing the wrong one I believe. This is the Boss post from the V9 CD? Anyway, for 3 place decimal, you need to change FS1 like so:

fs 1 1.3


This will output anything that uses FS1 to a 3 place decimal (like X, Y, Z moves and such).

To get rid of the "G70", in your 'psof' section, you'll have a safety line like this:

psof # Start of file for non-zero tool number 1001
".", n, "G70G75G90", e

Just remove the G70 or change it to the metric code you need.

Now, FS2 is for incremental data, so you'll want that to look like this:

fs 2 1.3i



Edit: Matt is quick!! I change my FS stuff, but Rek'd makes good points on what to edit and not edit..... If I need more, I just create more......

[Rekd]

Originally Posted by psychomill Edit: Matt is quick!! I change my FS stuff, but Rek'd makes good points on what to edit and not edit..... If I need more, I just create more......

I used to change mine too. Then I changed one that affected something completely different and didn't catch it in time. Now I create new ones and assign what I need to them. Much safer.

[Moorej91]

Thankyou everyone for your help. I will make the changes and let you know.

[Moorej91]

I have changed settings as you suggested and the machine works doing a contour path. It did come up with a Aborted- data verify error (bad data).

I then tried to do a 3d path but it moved in the xy datum when it should have been in the xz.

Is this to do with the settings? Can you tell me what to change?

Thanks for your help

Jeremy

[Rekd]

Sounds like you're in the wrong plane. You (typically) have to change the tool plane in order to contour in XZ/YZ.

Or you don't have the correct level to do 3d work. What ver. level are you using?

[Moorej91]

I am not new to 3d cadcam as I have been designing and machining for a few years now. I have been using mastercam V9.1 level 3 and know all about tool plane and know that it works. I normaly post to a hurco machine with no problems but following a breakdown, I am trying to get the bridgeport running until we can get it sorted out. A normal countour plane worked well, but on a trial "wave" shape to test the post it seemed to be working in an xy plane and not the expected xz plane.

I am trying to edit the post with the help of cnczone, this being my first visit and a new user.

Is it a post problem?

Regards

[Rekd]

Originally Posted by Moorej91 I am not new to 3d cadcam as I have been designing and machining for a few years now. I have been using mastercam V9.1 level 3 and know all about tool plane and know that it works. I normaly post to a hurco machine with no problems but following a breakdown, I am trying to get the bridgeport running until we can get it sorted out. A normal countour plane worked well, but on a trial "wave" shape to test the post it seemed to be working in an xy plane and not the expected xz plane. I am trying to edit the post with the help of cnczone, this being my first visit and a new user. Is it a post problem? Regards

If you've done 3d stuff with MC before, then chances are it's a post issue. Unless the Bridgeport controller does not handle 3axis machining.

[Moorej91]

Thanks again for your quick reply.

I have been doing 3d machining on our hurco and using mastercam, but I have not used the bridgeport for 3d yet. How can I find out if the machine will support 3d milling? As the machine does 3 axis cnc I assumed that it will do 3d machining. Is this not the case?

Regards

Jeremy

[Rekd]

Originally Posted by Moorej91 Thanks again for your quick reply. I have been doing 3d machining on our hurco and using mastercam, but I have not used the bridgeport for 3d yet. How can I find out if the machine will support 3d milling? As the machine does 3 axis cnc I assumed that it will do 3d machining. Is this not the case? Regards Jeremy

I'm not sure if that's the case or not, just trying to put as many options on the table at once to give you things to look for before I go home for the day.

[Rekd]

If you've got code samples for the bridgeport, compare them to your posted output. Perhaps all you need is a G18 or G19 instead of a G17.