Hello everybody….

This is my first post, I'm so glad I'm sharing this with you, I really need urgent help.

I have Cincinnati milling machine and I'm using siemens post processor to run it which I modified by my self, I run contour program, but I can't run circular pocketing on it, I'm using Keycreator CAM software.
this machine runs very well using a MASTERCAM post processor but I want to run it with Keycreator, I can send the post processor of MASTERCAM, and Siemens which I modified, if you can help me I'll appreciate it.

Thank you

M.M

Hi

I think you'd better to use surfcam for your machining g-codes .
also would you tell me how do you start machine and move the axis ?
however I need the electrical drawings would you kindly send them in .pdf format

Best regards,

Jalal

the cam system supplier should provide the post.

how to start the machine?? I assume you have the A2100 control. After it is wired and plumbed for air, turn the big black handle on the back electrical panel to "on". From there move to the front of the machine and push the green button on the operators console. Wait for everything to load up and when the operating screen comes up it will tell you the axes are unaligned. Look up at the remote pendant and push the align button. The readout on the pendant will show axes align and mech align. Push the button for axes align. If the table isn't close to home position, far right corner, you will have to hold it until it takes over and starts aligning itself. Once that is finished it will ask on the operator screen, if tool 1 is in position on the tool changer; tool 1 should be visible in the little window on the apron of the toolchanger and ready to swing over to the spindle. If it is, hit the button below mech align on the pendant readout and it's ready to go. Now you get to load the toolchanger and set tool heights.

One other thing, before you start running it or playing with it, make sure you push the button and the little red light for rapid override is on on the pendant. This will allow you to control the rapid movements with the feedrate knob on the pendant; these move pretty fast with it off and you will be scrambling to hit the Estop when things go wrong... and you will be too late.

Thank you very much Kccrusher, but I run the machine the problem is with my post processor, Im using Keycreator for CAM and any I, J format never works, but with MASTERCAM there is no problem with circular interpulation.
Anyway thank you very much this will help in a way or anothor

the starting of the machine was for Jalal.

On the post, I had the same problem with one of ours. To use it, I had to go into the machine configuration, the circular interp parameters and change it to always absolute I and J instead of the ability to designate either one, as it just wouldn't produce what I wanted and I didn't have time to play with it to get it to work, I needed it to produce parts! In the parameters you have the ability to switch to absolute or incremental only, or be able to toggle between both. Just be aware that you may be messing up any previous program that was programmed outside of what you set your parameter to, including using the RAP on the machine. Hope this helps.

The I and J Values Are absolute values On the Acramatic Control not incremental like a Fanuc Control Machine. Check your Post and make sure it is set to post absolute values for I and J.

not true; if you can access your machine parameters, there are three options to choose from in the circular mode concerning I and J values, incremental, absolute or both, i.e. must be specified in the program to which one you are using in the line.

Well I guess I learned something today I was unaware of this parameter and just have been Programming my 850 and 2100 Controls always using absolute values for I and J. The Sabre 500 with the 850SX control is 16 years old I am not sure if this is an option on this machine. So I guess it just depends on the age of the machine. The 2100 controlled machine is newer and this may be a possibilty but, If it were me I would just edit the post. So this way any excisting programs will still run.

Yes, you are correct; anything to cut time is good and making the post to where it is common to everything else you do is a winner every time.

I'm not familiar with the 850 control, just the 2100 and only enough to be dangerous! All of our VMCs use the A2100 control. If you have the password to get into the service area, that's where you will see this parameter; not everyone has that for their machine and when we purchased any of our VMC's that were out of warranty, we get it, as it's not always the same from machine to machine, as our technician changes it to his common password on anything he works on. I just keep it away from the operators, as it can cause problems when they change something, don't document it and another operator takes over on the following shift.