Customizing VCarve Pro and PartWorks

Well I know it’s been too long since my last installment, and I have a bit of a backlog of ideas to write about. I’d like to detail how I use VCarve Pro and my ShopBot to work with the RTA (Ready-to-Assemble) fittings, but there is something else I need to explain first. I’m going to show how you can customize the VCarve Pro (and PartWorks) postprocessors to get the specific outputs you want, then next time I’ll describe how I use these modified postprocessors to create toolpath files for handling sheet materials including using RTA fittings and the auxiliary drill head. So this installment is pretty much useless to you unless you use VCarve Pro or PartWorks, but it seems many ‘botters are using or are interested in these excellent programs so here goes.

It seems too few people realize that the VCarve Pro postprocessor files are text files which can be edited with any text editor program. (To clarify, PartWorks is the same program as VCarve Pro, but it comes with only the ShopBot postprocessors. For the purposes of this article, PartWorks and VCarve Pro are identical, with on exception which I’ll get to.) Our friends at Vectric are understandably hesitant to encourage us to fiddle with the postprocessor (.pp) files, since if you make a mistake it could lead to ruined material, broken tooling, damaged machinery, and/or personal injury. So please don’t tell them that I’m writing this, but if you are reasonably comfortable with editing .sbp files and understand what the various ShopBot commands look like and how they perform you should be able to successfully modify a .pp file to your liking.

First, be very careful when modifying a postprocessor file as every character makes a difference and the results can be unpredictable. Be sure to keep a copy of the original postprocessor file, or, as I do, save the edited file under a new name so the original file is kept unchanged. You can make the modifications in any text editor including the ShopBot text editor. The postprocessor files are found in the “Program Files\VCarve Pro 4.0\PostP” folder on your hard drive. You can name the new file whatever you want – the name of the file will not affect the performance or even be visible while using VCarve Pro. For simplicity’s sake I’ll use as an example the “ShopBot_alpha_Arc_inch_router_control.pp” file – others may vary slightly but should be similar enough to follow along. Open the file and familiarize yourself with the layout and contents. Any line that begins with a “|” or a “+” character is a comment line and is there for information only. So you can see the first paragraph is a list of the authors of and contributors to this postprocessor file and the dates on which their contributions took effect. Go ahead and add your own name, date and the changes you are making so you’ll have a record of your work. Just remember each comment line has to start with a “|” or a “+”

Just after the first section of comments is the line:

POST_NAME = "Shopbot (arcs)(inch)(alpha_control)(*.sbp)"

Whatever type is between the quotation marks in the above line is what will appear in the postprocessor drop-down menu when you go to save a toolpath file in VCarve Pro. I suggest changing it to something short, sweet, and descriptive, such as “Plywood” or “RTA fittings”. You do not need to include the (*.sbp), but don’t forget to leave the quotation marks. (Here is the exception for PartWorks users – you will have to have the name “Shopbot” included somewhere between the quotes.)

The next several paragraphs are used by VCarve to set variables which will be used later in the file. I have no idea what most of them are for but some of them are obvious and if you are sure that they will not be used in the final postprocessor file than you may safely delete them. For instance, if you do not need to set the spindle speed from within the resulting .sbp files, you can delete the following section:

+ Spindle Speed
var SPINDLE_SPEED = [S|A||1.0]

If in any doubt about any line or section, just leave it be, it won’t hurt to leave it in.

Farther down the file you’ll find a section that begins with this:

+ Start of file +
begin HEADER

followed by a bunch of commands and/or comments. Whatever follows the above will appear at the beginning of each file which is output using this postprocessor. Since I use a master file to call all my sheet cutting and drilling files in the proper order and to control things like cutting speeds and turning the router on and off, I simply delete this entire paragraph for most of my .pp files. But if you want any particular commands or comments to appear at the start of each file, this is the place to make that happen. Notice that each line starts and ends with a quote mark [ “ ] which will not appear in the resultant files but cannot be left out. Note also that this is where the commands are generated that send the tool to the “home” position at the beginning of each toolpath file, so if you want to eliminate that pesky feature (like I did) just delete the line:


Here’s a hint: If you replace everything after “begin HEADER” with the simple line:


Then the command C5 (Custom Cut 5) will appear at the start of each .sbp file output with this postprocessor. You can then save any standard start-of-file commands as a Custom Cut file (Custom5.sbc) and it will be run as a subroutine by each file before starting the cutting moves.

Next, look for the section that starts with:



Let me digress here for a moment. One of the benefits of learning how to modify the postprocessor files is the ability to create .sbp files that perform a specific task or function at each vector location in your drawing, instead of the cutting action which VCarve thinks it is creating. Specifically, if you use a Drilling toolpath on a group of circles, you can substitute the code of your choice in lieu of a Move command in the postprocessor file where VCarve thinks it is going to drill a hole. For instance, you can use the CC or CP commands to drill a hole with a spiral plunge, the C# command to invoke a custom cut file, or even the FP command to run a particular file at each hole location on your drawing. This last sentence is the key to my technique for machining holes for RTA fittings with VCarve Pro, which as I said I intend to cover in more detail in my next installment.

So back to our file. The following line is the move command that will be generated for each required move. If you are just tweaking your router or spindle .pp files to adjust the headers and footers you’ll probably want to leave this alone, but to change the function dramatically try replacing this entire line:



“FP, RTA fitting.sbp,,,,,2” (0r substitute the name of the file you want to run at each hole location.) Don’t miss the five commas followed by “2” – that specifies that the named file will be run in 2D offset mode.

Do the same thing where the file says:

begin FEED_MOVE 


Now the resultant .sbp file will move the machine to each hole center location, and run the indicated ‘RTA fitting.sbp’ file (or the file or commands of your choice)

If you’ve made it this far you can probably decipher the rest of the postprocessor file. For my RTA and drilling postprocessors there are no “arc” moves – or any other type of moves needed so I just delete the entire rest of the file. If you are just tweaking your cutting postprocessor you can adjust what happens at the end of each saved .sbp file in the section just after the line:

begin FOOTER

Again, substituting the original lines of code with a C# (or FP) command will let you run a standard end-of-file routine at the end of each .sbp file.

Once you are reasonably sure you’ve correctly modified your way to a new, improved postprocessor file, save it with a .pp extension in the same directory mentioned above. Then open VCarve Pro (or PartWorks). The software actually scans each postprocessor file upon opening, so if there are any obvious syntax errors you will get an error message right up front, with a line number that corresponds to the line number in the .pp file, which gives you a place to look for the problem. If the software starts up OK, then try saving a toolpath using your new postprocessor. Make sure to check out the first few resulting .sbp files with a text editor to be sure there are no surprises, and run the first few files in preview mode just to be sure. Since I started using my modified postprocessors I rarely if ever have to edit or even check my .sbp files before running them. Here’s another tip: you can delete or move to a new folder all the .pp files for any machine you don’t currently own and don’t expect to own any time soon. Do the same for any stock .pp files you won’t use, such as metric files if you only work in inches. That way when you go to select a postprocessor file in order to save a toolpath you’ll have a custom menu of all your own .pp files with no unnecessary extras. (You can restore the original .pp files by re-installing VCarve Pro.)

Sample files: The attached files are meant as samples only, although you can use and/or modify them as easily as the ones which come with VCarve Pro. For each .pp file, I used VCarve Pro to toolpath a simple drawing consisting of four small circles placed at 2,2; 2,4; 4,2 and 4,4. For the RTA Only file I used a Drilling toolpath with the depth of cut set to zero; the resulting .sbp file runs my “RTA fitting.sbp” file at each hole location.

For the Custom Cut file I used the same four circles but a Profile toolpath and a .5” depth of cut. The resulting .sbp file has a C5 command as the Header and a C6 command as the Footer, with the typical machine output in between. If you use the C#, format you can use Custom Cut files with 2-digit numbers and keep your single digit numbered Custom Cut files for use with the keyboard.

Comments are closed.