PC2100 Post

[treej250]

Is there more than one post processor for the Acramatic PC2100 control? I cant seem to make the only one that comes with MasterCam work. It will post out fine, but when I run the program on the machine I get an error message at a arc move. G2 or G3.

thank you.

Mark

[ERIC14779]

Are you getting a invalid point or equivilent. If you are it may be that your machine is in 4 place accuracy and the post is outputting 3 places after the decimal. I had this problem on my Quintax 5-axis with a xxxxor 8055 control. The post I was using was set to output 3 places after the decimal and the accuracy perameter in the CNC was set to .0005 so a rounded 3 place coordinate was out side of the alowable error.

I modified the post to output 4 places after the decimal and all is well on G2 and G3 moves

[treej250]

You may be right. I do notice that all the digits on the control for X, Y, and Z are to 5 place decimal accuracy, and the post is outputting to 4 places. I wonder why my control is showing 5 places after the decimal? I cant machine that close.

Mark

[ERIC14779]

Your machine factory service person for the machine should be able to help you change your CNC control to display and handle 4 place decimals with out the rounding error.

I belive this will eliminate the error

hope I helped

Eric

[Allan]

PC2100 great control wierd arc stuff. There is a setting in the machine for arc centers I can't rembember how to get to it but the thing will switch from incremental arc centers to absolute centers based on the G90 G91 in your code! You'll want to change that to always incremental.

Allan

P.S. The mpmaster.pst from this site has the correct helix stuff in it for the PC2100

[ferdelance]

i have a few ideas for you.

1) the control shows numbers to five decimals but that doesnt affect your programming.

2) on your control, go to machine applications/cnc programming/...there is a choice there for report cdc errors, make sure that is turned on...then under the circular page, there is the option for end point tolerance, make sure it isn't set to something rediculous.

3) you can't use p's and q's for cdc unless you purchased that option and turned it on, so make sure you are using g40/g41/g42

can you post the lines for the interpolation?

hope this helps

oh, btw, g90 and g91 is a matter of choice when programming for the 2100, depending on what you like and what makes things easier for you...mho

[ 08-21-2001: Message edited by: ferdelance ]

[mikee]

I was told by Mc to also try the mpvickers pst a while back.

mikee