The MPOST Post Processor Package

The other post processor package shipped with SURFCAM contains three post processors: MPOSTWIN used with mills, LPOSTWIN used with lathes, and EPOSTWIN used with wire EDM. Each is an EXE file. (For simplicity we often refer to all three as the MPost post processor.) These programs are stored in the SURFCAM\Surf2003\MPost folder. The post files for this post processor package are located in the SURFCAM\Postlib\Mpost folder. The name of each post indicates the manufacturer, the model name and NC machine type. For example, CIN850.M3 is the post for a 3 axis mill made by Cincinnati Milacron. The model number is 850M.

To get machine configuration data, the post processors MPOSTWIN, LPOSTWIN and EPOSTWIN read the corresponding “POSTFORM library” files POSTFORM.M, POSTFORM.L AND POSTFORM.E. These are text files that contain copies of several posts that you want to have readily available. The post processors read the POSTFORM files to get the post names and display them in a menu. You select the post you want and the post processor goes to that part of the POSTFORM file to get the machine data it needs.

By using a text editor—such as the SURFCAM editor—you can add posts to, or delete posts from, your “POSTFORM library” files to make them better fit your needs.

The first line in a post file contains the word “name” followed by the name of the post. The file can be several pages long. The POSTFORM files consists of the contents of several post files appended together. To add a post, append the contents of the post file to the POSTFORM file. To delete a post from a POSTFORM file, delete the “name” line for that post and all the following lines up to the next “name” line.

Creating an MPost Post File

IF the SURFCAM post library does not contain one of these earlier posts for your machine, you can create one. SURFCAM is shipped with two post template files:  Generic.M and Generic.L. These files contain a set of quasi-standard characteristics for mills and lathes. By taking the machine characteristics provided by the manufacturer, you should be able to modify one of these generic post template files with a text editor to produce a post for your machine.

Running an MPOST Post Processor

These post processors are run from the NC Operations Manager dialog box.

From the NC Operations Tree, select the NC operation or set of operations you want to post process. Then double-click List All in the NC Post List box. This will display a menu of the available posts.

Specify the machine tool by clicking on its name and number. Then click OK.

Depending on the post you select and the parameter values you enter in the Tool Information dialog box, a series of additional dialog boxes may be displayed prompting you to enter additional data. The following examples prompt you to enter values for work offset number and program number.

After you have responded to any prompts for additional information, the post processor will create the final NC code—using the data from the toolpath file(s) and the post—and save it as an NCC file with a file name that is automatically assigned by the NC Operations Manager. This newly created NCC file will then automatically be loaded into the SURFCAM editor and displayed on the screen.

You can now modify the NCC file, if needed, and re-save it. If the assigned file name is not acceptable, now is the best time to use the Save As command to assign a more useful name.