There are many times when our computer controlled machines seem to have been taken over by gremlins.  Usually, these “gremlins” are erroneous settings that cause unexpected actions in the machine, or unexpected reactions to commonly used commands.  Windows (all versions) has long been plagued by errors that occur when the OS is closed abruptly.  The same is true for most Windows software.   SB3 and the SB Link are no exceptions.

Since ShopBot 3 and the ShopBot Link both require a large number of settings be stored accurately to enable our machines to operate properly, keeping a backup copy of these settings is essential to a quick and painless recovery from a software crash.  There are a number of causes for these crashes, many are a result of external electrical charges, or in some cases, the machine has hit a limit switch or experienced a power surge or flicker.

Without going into what can cause these crashes, I will show you how to recover from them and be back up and running in a few minutes.  Of course, before we can restore from a backup, we must first create a backup.  Here is the method I have shown to a good number of users.  There are many ways to accomplish these simple tasks, this one uses Windows Explorer and select, copy and paste mouse commands.  On some computers, you may have (or wish) to select these commands from a menu or drag and drop instead of using a mouse click.  Use the method that you are the comfortable with.

Note: In cases where a user would call ShopBot Tech support, they will ask you to install the latest version of the software and proceed as per instructions.  This method gives  Tech Support a known baseline that will allow them to repair most software related problems.  Installing a new version of SB3 overwrites many of the settings and customized files we users have stored in our machines.  My method allows us to keep our current software version, all of our custom settings and files intact, and should take less time than a call to support.

If you are not comfortable using Windows Explorer to copy and paste files have someone help you, as it is important to get this right.  This procedure cannot replace tech support for all users, but in cases where the user has fairly competent computer skills, will allow him/her to self repair without a great deal of effort.

Create a Backup:

Open My Computer > Double click to open “C:” drive  (may be named something like C: “special name”)

Select C:\  then R click and create new folder, name “BACKUP” or “ZBACKUP” to have your folder displayed at the bottom of C:\ drive contents.  If you have multiple drives on your machine, locate the BACKUP folder on one other than C:\.

SB3 Control Software:

Find (if you have saved a local copy) the SB3 version that was used to install your current Control software.  For example the latest version is named: “Setup_sb3_6_38.exe”.  Once located, R click and select copy.  Navigate to where the BACKUP folder is visible, R click and select paste.  Verify that the file has been copied there.  You can download the SB3 software, but I prefer the speed of a local copy.  Saving a local copy also keeps you from forgetting which version is your “known working”.  When downloading a software version from the ShopBot website you have the option to “Save As”.  Navigate to your BACKUP folder and save your preferred version there.

SbParts Folder:

With the C:\ folder open, R click the “SbParts” folder, select copy.  Navigate to where the BACKUP folder is visible, R click and select paste. Verify that the file has been copied there.  You should repeat this copy/paste (select overwrite) anytime a change has been made to the software, your custom files or setup. A routine should be implemented to backup these files at least once a month.

SB3 Settings:

The next step assumes that SB3 is running, all your settings for speeds, ramps, homing (via the SB Setup), etc. are to your liking AND your machine has been homed and sitting at the 0,0 location.  Do not make the SB3 backup unless your machine is working error free.

From the SB3 Console enter [U]tilities [S]ave Current Settings to a Custom Settings File.  In the Save dialog box, navigate to the C:\BACKUP (or your other location) folder and save the file as, in my case, “GC SB3 Settings.sbd” Use a name that you will recognize as your SB3 software settings.  This file will store all your current settings, most of which we users do not know exist.  Make sure that the proper file extension is not overwritten.

IF you are a not ShopBot Link user, skip the next section and go to the “Restoring Your Settings” paragraph.  For Link users, the procedure is similar to SB3, but has an extra step:

SB Link:

Like SB3, make sure that your Link Settings are as you prefer them and are working well.  I usually go into the [Load] dialog and select [Clear All] to remove any parts loaded, but this is not important.

From the main screen, press the [Export] button.  Navigate to the C:\BACKUP folder and select [OK].  A command window will appear, the file is created, and you will be prompted to “press any key to continue”.  The name of this file cannot be modified during the save procedure, so navigate to the C:\BACKUP (or your location) folder, R click on the file named “ShopBotLink1-0-xx.cab” and select rename. (xx refers to current Link version)  Rename this file, in my case, “GC Link Settings.cab”, in yours, select an appropriate name for you.  Make sure that the proper file extension is not overwritten.

Restoring Your Settings:

In most cases the control software does not need to be reinstalled.  IF you feel that it does, remove the current version using  Windows Uninstall.  The path to this varies a little between versions, but “Add or Remove Programs” or “Programs and Features” are located in the Windows Control Panel.  Select “ShopBot 3 version 3.x.xx” from the list and press “Uninstall”.  You may choose to skip this step, if so, proceed to “SbParts:” below.

SB3 Control Software:

Once Windows has completed the uninstall procedure you may want to reboot the computer and possibly run a registry checker to remove or repair any errors.  Next, navigate to your BACKUP folder, double click on the “Setup_sb3_x_xx.exe” file to install SB3.  For this install it does not matter which of the install options you select as we will overwrite all the OEM with your saved files.

SbParts Folder:

Next, navigate and open the C:\BACKUP\SbParts folder.  R click and select all (or [Control] + [A]), R click and select copy.  Now navigate to the C:\ drive, R click on the SbParts folder, and select Paste.  When prompted, select overwrite or replace, depending on your windows version.  I have a trimmed down version of SbParts with no OEM files in it.  I usually delete all the existing prior to paste of the backup files.  Unless you have a large number of modified files, you can skip this step.   You should now have a clean version of SB3 installed and have kept your user defined variables and customized (if any) files.

SB3 Settings:

Turn on your machine, Start SB3, square the gantry, zero the X & Y axes (home) and leave (or move) the cutting head at (or to) the 0,0 location.  From the SB3 Console, enter [U]tilities [R]eset Default Settings, Load……  Select [YES] to the “Do You Want to Clear the System Log….” dialog box.  Select [Yes] to the “Do You Want to Load the Default Settings or Load a Custom Settings File……” dialog box.  Select [OK] to the “Select and Load Settings….” dialog box.

Navigate to your BACKUP folder and select the “Your Saved Name SB3 Settings.sbd” file.  SB3 will load all those settings that were saved when you made the backup. SB3 Settings are done.

If you are not a SB Link user, you are done and should have a machine that responds as expected.  Once you go thru this process a couple times you can accomplish it in a few minutes, and knowing how to do this may save you a good number of calls to SB Tech Support.

SB Link Settings:

Open the SB Link, and from the main screen press [Import]. Navigate to your BACKUP folder and select your “Your Saved Name SB Link Settings.cab” file.  That’s all there is to it.  You are good to go.

In most cases this will repair lost or erroneous settings caused by a software crash.  In the cases that it didn’t, you will most likely have to install the latest version of the control software and possibly call support.  In other cases there may be a bad component or computer problem that these settings fixes cannot repair.  In any case you still will have the ability, once your machine is up and running, to cherry pick Custom files, variables or user modified files from your backup folder.  When doing this, make sure you save the existing OEM file with another name, in case there is a problem with your backup version of that file.

If you are able to diagnose that your problems are isolated to either SB3 or SB Link settings, you can restore those settings alone, but if you are not able to diagnose and isolate which is the cause, Follow the steps above, In Order!

Winter, and its never ending supply of static making dry air is almost upon us.  Hopefully, this procedure will give you a way to recover from software crashes caused by this static and some of the other gremlins that make our ShopBotting experience not so fun.  I would recommend that if your experience these problems more than once a month, that you make a concerted effort to find and repair the root cause.  You can also save your BACKUP folder to a thumb drive and use these files to allow another machine to have the exact settings as your original.

Hopefully, this will allow you to get up and running quickly after a crash and truly have a “5 Minute Software Fix”

(Note: Many versions of SB3 software contain improvements over the previous versions.  This method does not allow you to take advantage of these improvements)

My blanks have been glued up in a jig and trimmed to ensure consistency. I drew a recess .030 larger than the blank in VCPro and cut it into the Spoilboard. This allowed both some sorely needed Z clearance and indexed the parts at a known location. Additional pieces of scrap were used to complete the holding portion of the jig.

With my exact location known(rectangle from 5,6 to 35,12) I drew the radius for the concave face. The radius was 150”. To do this I placed a circle with a 150” radius with its center at 20 (center of the blank ) in X and at 148.5” in the Y. This gave me approximately 1.5” negative in the arc portion I was going to use for the toolpathing. I then placed 2 lines vertically at X=5 and X=35 and trimmed away the majority of the circle to them. Then deleted the 2 lines. I now selected the arc and moved it so that the top of the arc was at Y=0. This is the exact profile that I need.

In order to have a small leadin, I placed a ½” line at each end of the arc and raised the outer end to a height of .010. All 3 sections are joined and I have a completed cut vector with a small lead, ready to toolpath. I selected the vector, entered node editing mode and noted its start point. In my case it was on the left. Exit node edit mode, select vector and made an ON vector toolpath with a Vcarve bit, to a depth of -.1235. This depth or the bit selection is not important, but you need to select something that will be easy to spot in lines of code. Once this toolpath was calculated, I node edited the start point to the other end of the vector and calculated a similar toolpath in the opposite direction. Here is a screenshot of the node editing and toolpath versions of the vector. Note the short leadins and start points in the node editing mode, and the cut direction in the 2 toolpaths.

The toolpaths were saved separately as “Plus X Pass” for the left to right, and “Minus X Pass” for the right to left. It is important that you only use the SB INCH post processor, as it will generate a number of short line segments for the arc. Any of the ARC INCH posts will generate a gcode arc for this movement and this will not be read by the Z. Here is a video showing how and what I did inside these 2 files to turn an arc that had it length in the X, and an arc’ed Y value into a file that rasters in the X, steps over in the Y and produces a concave Z action in the Z, similar to what a 3D toolpath would do. There is also a short section on the master file that runs these 2 passes back and forth.

Before I place the code for the master file for you to copy and paste, you must acknowledge that these files were made for my machine, and even tho have worked, may not work on your machine. Also note that modifying a parts file without proper knowledge could cause unintended machine actions and do bodily harm. Please use these files at your own risk.
Here is a picture of the legs, in the booth, after sanding sealer was applied. Note how the color appears to change at each corner due to light refraction differences between side and end grain. Finish is clear.

Master File:
‘File created in VCarve or Aspire
‘File Created for Islamorada Woodworks
‘UNITS = INCHES
SA ‘set to absolute mode
‘++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

&step = .05
J3,6,0,.125
MS,6,2
TR,13000

BEGIN:
&count= 0
PLAY D:\SbParts\Bell School Traditional.wav
SO,1,1

J3,4.0,5.75,.125
&y_value = 5.75
PLUS_LOOP:
&y_value = 5.75 + (&count*&step)
MY,&y_value
FP,D:\SbParts\Walnut Legs\Plus X Pass.sbp
MX,36.0
&count = &count +1
MINUS_LOOP:
&y_value = 5.75 + (&count*&step)
MY,&y_value
FP,D:\SbParts\Walnut Legs\Minus X Pass.sbp
MX,4.5
IF &y_value > 12.2 THEN GOTO DONE
&count = &count +1
GOTO PLUS_LOOP

DONE:
JZ,.125
SO,1,0
JY,15
JX,50
JY,0
MSGBOX(CUT ANOTHER SIDE?,YesNo,REPEAT)
IF &msganswer = YES THEN GOTO BEGIN
END

Simply said, your zero location should normally be between the table and its upper limit of travel. If you have 6 inches of travel, then you cannot zero higher than 6 inches or below the bed. There are of course, other factors, but for normal cutting, these are the upper and lower limits.

Now for the relativity. Unless you have the world’s best eyeball, you can’t actually zero to the bed or an object, you zero to the Z zero plate. The control software has been told the thickness of this plate and it sets the position that it electronically senses (the top of the plate) as that thickness. The actual zero position is set relative to the top of the plate, by its thickness, to be the bottom of the plate. The same logic applies to fixed zero blocks. Its position, relative to the table surface, is adjusted for in the software during the zeroing routine.

Contrary to popular belief, zeroing a bit to any plate or block is very seldom exact. Due to electronic timing, the downward motion does not always stop at the exact same spot every time. Some bits dig into the plate. The plate can bend or have a low conductive spot on it. The bit can be coated. Individual control boards can react to the input signal with minute variations. All of these items can result in a few thousandths variation of position. Even more if one or more of them add together instead of canceling each other out. In most conditions, you can expect 10 thousandths either side of zero as the norm, 5 if you do some tweaking of your zero file and procedures.

These minute variations rarely affect our cutting until we wish to do a pocketing operation with multiple bits. Although irritating, it is common to see a second bit cut at a different depth. As users we need to develop methods to check for inaccuracy prior to cutting.

These electronic variations are nothing compared the variations in most processed materials, especially sheetgoods. It is not uncommon to see 30 to 40 thousandths thickness difference in a single sheet, even more across multiple sheets. More yet in inexpensive imported products. Our problem as operators is to find the actual or average sheet thickness from edge measurements. I usually take multiple measurements and average them to get my design thickness. In many cases, I have had to readjust the sheet thickness after cutting to reflect the actual material thickness in the interior of the sheet where my parts are cut.

Most sheetgoods cutters zero to the bed because we seldom know the real thickness of the material in the selected zeroing location. There are also variations with hold down due to material porousity. Prefinished and melamine are sealed, allow more vacuum to develop and therefore, suck down tighter than unfinished veneer plywood. Once a sheet is on the bed, should any problem, like position loss or broken bit occur, it is virtually impossible to rezero to the Spoilboard without removing the sheet. This is why most cabinet cutters use a fixed zero block, usually off the one end or side and below the surface of the Spoilboard so that it does not interfere with table surfacing.

The points that apply to the majority of users are this: Unless your material has been surfaced by the CNC you cannot assume that it is flat. Nor can you know the actual thickness at the zero location. These two facts added to the above electronic variations are the reasons for most of the depth inaccuracies facing small CNC users. There are also a number of variables associated with spoilboads, but we can save those for a later day.

As likely as a sheet cutter is to zero to his Spoilboard, most other users are not. There just seems to be something “off” with the way that most CAM packages treat zero to bottom of material. My experience is that it is harder to learn and more prone to error. Maybe it is just that we are programmed to think from the top down into the material. Even though I tested a number of files, my results were less than satisfactory and I followed the masses and prefer to design from the top.

I wanted the extra accuracy that zero to the bed gave me, but I also wanted the ease of use that I was accustomed to with zero and design to the top of material. There is a third way that allows both. Allows me to zero to my Spoilboard and then check the bit height against the Spoilboard in multiple locations prior to cutting. It also allows me to design my cutting files from the top of the material. It allows me to cut different thickness materials without a rezero of the bit. This method ensures that my actual bit zero is at the design thickness of the material. It does not eliminate errors cause by variations in that material, but will keep all other variables to the bare minimum.

I learned about this while beta testing for the ShopBot Link from the Thermwood programmers. Their files are all zero to bed, design and cut from the top. With their help I was able to understand the principle and implement it into my own Vectric post processors.

Here’s how it works:
The Vectric Software outputs the design thickness of the material to the post processor. The PostP, using some of the new features of the SB3 software applies a temporary offset called the “ZSHIFT” to the Z axis for the duration of the cutting file. When the file is complete the offset is removed. For the duration of that file, the Z zero is actually at the top of the material. If your next file uses the same bit, but a different material thickness, no rezero of the Z axis is required. The only time a rezero would be required is when a bit is changed.

So…. My theory is that the Z Zero should be automatically relative to the material thickness. Here is a screenshot of the Vectric material setup dialog showing that zero to top is selected. The red lines show the offset that the ZSHIFT applies.

This feature works with both MTC and ATC files, but may not be in the mainstream files distributed with the SB3 software. As such, it is most likely not supported by ShopBot. This means that you either need to be or know someone that can modify your post processor. Or, you can borrow a copy from someone that is using it. Although very seamless when installed, there is a certain amount of expertise required to modify the post and implement the changes. And did I mention no tech support? Enjoy!

Parts on Table Less Pipe

In order to be able to implement a large blower in the future, it was obvious that a valved distribution manifold was in order, even though a less costly vac source would be used short term. My primary objections to the manifolds I have seen are 1) PVC ball valves are hard to operate and seem to get harder with extended use and 2) the plumbing and fittings required to make these valves accessable add to the cost, complexity and restriction of the system.  We now have our design criteria for the manifold system, no PVC ball valves and Keep It Simple, Stupid!

Thru Pipe Glued in and Rounded Over

I decided to use 2” knife valves instead of ball valves. Advantages of these valves are: 1) they are equipped with O-ring seals, 2) seals are replaceable, 3) the actuator handles can be extended to allow remote valve placement with up front control. The only disadvantage is that they cost a few bucks more.
Our plenum was designed as a 49 by 97, 4 zone, very typical to many I have seen. We cut the vac holes thru the table with the ShopBot so that a piece of pipe would glue in directly, eliminating flanges or fittings at that location. We used Corian adhesive for this connection. After the adhesive cured the top of the pipe and plenum were radiused using a 3/8” roundover bit.

Under Table View Showing Valves, Rods and Dump Valve

The manifold was constructed using 2 double outlet wyes and 45’s for the branches and a 3” main trunk. A 3” knife valve was installed to allow a quick dump of vacuum for both rapid part changes or emergencies. We plan to add an air cylinder controlled by the software for this valve in the future. The 4 zone valves are installed directly under the vac holes just low enough to allow the extended control rods to pass under the table supports. These extensions were fabricated from ¼” aluminum rods and fastened to the valve using bolt couplers. Holes were drilled thru the 2 center leg supports to allow the rods to pass thru. Holes were also drilled into the table support on the –X end for valve handle placement. After all extension rods were in place, they were marked, removed and had threads cut for the handles. Handles were installed with lock nuts.

End View Showing 2 zones Open and 2 Closed

The final picture shows a front view of the machine with the vac manifold installed.  You have to look carefully to see the handles, let alone any of the manifold piping.

For the full sheet index, I don’t need something extremely accurate, but the system has to be able to withstand hundreds of sheets being slid into and against it. I also wanted something that would virtually disappear when not in use. I chose pancake cylinders for this as they have a 5/8” shaft and are very tough. I have used standard cylinders in the past, but have found the shafts to be too flexible when extended to give reliable accuracy. To ensure that the 2” stroke versions that I had on hand would reach above the Spoilboard from their under the table mounting location I extended the shaft with a 5/8” bushing cut in length and bored on the lathe to accept a mushroom head cap screw. Here is a picture of a cylinder, ready to mount under the table:

You can see the holes for the piston and mounting bolts next to the cylinder. Note the extension bushing and bolt added to the piston. I cut 3 sets of these holes with the Bot. Due to table framing, these were centered at 6”, 32” and 70” in the X direction and at -.3125 in the Y. This puts the edge of the 0.625” piston at zero in the Y.
Since these are dual action cylinders that use air to move both up and down, I used a 4 way, 5 port valve to operate them. A 5 port valve has a pressure port, 2 switched ports (1 for up and 1 for down) and 2 exhaust ports. Here is a picture of the valve with one touch fittings installed:

I installed the valve into the corner brace near the 0,0 corner. Here is a picture of the installation with the pins up and the valve installed:

To accommodate our smaller parts and the Flip Ops, I decided to make an “L” shaped fence from plywood that, depending how it works, will be made from acrylic or aluminum later. I drew an oversized version in VCPro, and cut it, along with 2 holes .005 oversize for the pins at 6 and 32. I also made a single vector toolpath to trim the fence to 3” in both the X and Y. I also added a corner relief to allow for chips and splinters. Here are screenshots of the Fence cutout and the trim toolpath:

Trimming the oversized fence after it has been installed on the pins assures both positional accuracy and squareness of the fence. In my case, both the X and Y position is 3”, but any number can be used. To use this fence for Flip Ops with the SB Link, all that is required is to add those coordinates into the Link’s Flip Op fence location.
For VCPro cutting files, adding 3” as a 2D offset into both the X and Y boxes of the fill-in sheet is all that is required. Parts are designed at a normal 0,0 position. You could also place the parts with the corner at 3,3, but my personal preference is to use 0,0 and the offset. The 2D offset feature allows us to change the location of the fence at a later date or trim it if damaged. The picture below shows the fence in place, after trimming.

Since we have used variations of these indexing fences for a few years, here some additional uses that have not been mentioned above:
In conjunction with disposable plywood zone masks placed tightly to the parts, helps stop parts from sliding.
By using holes bored into parts or their borders, a part that is larger than the table can be moved and repositioned onto other pins for second half cutting.
Long parts can be very accurately positioned at the Y=0 edge of the table.
For repetitive work, parts holding jigs with pin holes in them can be used interchangeably as needed.
I am sure that after using your version of this versatile accessory, you will come up with a myriad of uses.

Next Month: Vacuum manifold…. Have I ever said how much I hate plumbing?

If you have an accessory such as a drill or second Z added to your machine you will find even more uses for storing daylight values of different tools in each of your axes. If you have multiple Z’s and/or drills the advantages become exponential. Another advantage is being able to zero all bits to the spoilboard and have the post processor add the material thickness to the file as an offset. This will allow you to change and re-zero bits off the material to a location on the spoilboard. This can add accuracy and eliminate errors caused by zeroing to an area that is removed before a second bit is installed. It can also eliminate errors caused by materials that bow or warp during removal of material between roughing and finish passes. Drill users can eliminate the use of the drill offset file after a bit change by using a simple formula that compares the daylight value before and after a bit change. Having an upper limit allows lifting the Z to its maximum height to clear clamps and other obstacles on the table.
Even though most of the real work of the Daylight Method is done behind the scenes in the SB3 software, you will have to add a proximity switch to your Z (and A if you have one) axis. For the PRS I highly recommend the version sold by ShopBot. These prox switches have a long wire and have been specifically manufactured to be compatible with the newer control boards. PRT models use a different configuration and there are a number of good sources for them. You will need to fabricate a bracket that places the prox trigger point about 1/8” below the hard stop at the top of the Z travel. Here is a picture of a prox switch and trigger bolt mounted on my machine:

Mounting a prox switch on the vertical axis allows the same positional accuracy for the Z that we have for the X and Y axes.  The X Y zero routine uses stored offsets to set the 0,0 location.  The daylight method uses the same principal to record the distance from the prox to the table surface.  This is accomplished by “bumping” the prox switch after a bit zero and recording that value to the my_variables.sbc file.  This is the file where all similar values specific to your machine is stored. I used the syntax from the Zzero file to lift the Z axis to the prox and record the height.  Here is an example that works on my machine, but care should be taken to adapt this to yours:

LIFT_Z:
     ON INPUT (7,0) GOSUB TOP_Z             
     JZ,12                
     PAUSE .1
     RETURN

TOP_Z:
     ON INPUT (7,0)
     PAUSE .1
     &z_top = %(3)
     Pause .1
     MZ, (&z_top – .5)
     RETURN

After the “&z_top” variable is stored then it should be “written” to the my_variables file.  Here is an example of a subroutine that follows the syntax of the drill offset file and writes the stored variable to the file.  Note that the variable must exist in the file prior to this sub being used.

WRITE_TOOLS:
&name = “c:\SbParts\TempVar.txt”
OPEN &name FOR OUTPUT AS #1
WRITE #1;”&z_top = “; &z_top  
CLOSE #1
PAUSE  .5
Shell “C:\SbParts\Custom\MyVars.exe c:\SbParts\TempVar.txt”
PAUSE .5
RETURN

If you were to use the above action after you zeroed your bit and wrote the &z_top variable to your my_variables file, if you lose Z position you can recall the &z_top height and apply it to the Z location the same as you apply your stored offsets for the X and Y.  This would be as easy as writing a file to bump the Z against the prox and lowering .5” like above and then, using the VA command, assinging the value of  “&z_top-.5) to that location. 

 If you use a lot of fixtures and clamps to hold irregular materials as we do, you can use the prox to ensure that the Z is lifted to its maximum height for rapid moves, or even a Jog Home.  We have included this “Lift  Z and A” into may of our custom routines.  Some examples are:  The beginning of our warmup file, before we zero the X & Y and before we send the gantry to our park location for sheet change during sheet cutting.  I am sure there are as many variations as there are ShopBotters that implement the prox.  In any case, I am sure that it will be a valueable tool for all that choose to use it.

Tool Numbers:

Unless you have a ShopBot drill installed on your machine, you probably have not had to pay any attention to assigning a proper tool number to a bit that was installed on your machine. Even if you plan on using a single head and single bit, the ShopBot Link will require assigning a unique tool number to this bit. This is done in the TOOLING section of the SB link setup. Setting these up is very similar to any toolpath operation with Part Works software. Those of us that have drills already know that you must select the proper tool number to allow the software to apply the proper offsets for that tool. This will apply to all tools used with the ShopBot Link.

The numbering system that ShopBot has implemented uses tool numbers 11 thru 19 for head 1 (Z), 21 thru 29 for head 2 (A), 31 thru 39 for drill 1 (on Z) and 41 thru 49 for drill 2 (on Z), 51 thru 59 for drill 3 (on A) and 61 thru 69 for drill 4 (on A). Any consistent numbering system can be used, but the tool numbers selected in the TOOLING section of the SB Link MUST be the same as assigned to the proper head in the toolchanger routine.

Zeroing Using the ShopBot Link:

 To use files generated by the Link, you must zero to the top of the spoilboard. The Link outputs the material thickness for each sheet based on your design thickness and pre-nest adjustment, and the toolchanger files adjust the Z height based on this thickness. Another setting in the Link is for a “Wasteboard Thickness”. If you do not use an additional sacrificial board (most ShopBotters don’t) set this to zero. Any setting other than zero will bring up a message box with each sheet so that you can renter each time.

Custom9:

 Most of the “action” of the toolchange happens in the C9 file. I will try and explain what commands are required, how to make them work, and in what order to place them. Thanks here go to ShopBot’s Beta and Link Staff for their patience as they taught me these commands and functions as we Beta tested the ShopBot Link. Here is some sample code from the MTC file that swaps to the head 2 (A axis):

(First axes are set to equal height to allow swap)

VI, , , , , X, Y, A, Z

VO,1,&head_2_X_offset,&head_2_Y_offset,&z_adjust

The VI command sets the axis order to X,Y,A,Z which swaps the order of the A & Z and sends all Z height moves to the A axis. The VO command parameter “1” sets temporary offsets “ON” and applies an X offset, a Y offset and a Z offset (the material thickness) to the position. The X & Y offsets are the same number value that is used in the OEM inch or mm Head2 offsets, but you must be careful of the + or – sign. Between the PRT and PRS there are many different options to locating the 2nd head. To work with the toolchanger files, the proper value, negative or positive, can be best explained as the position that the head 1 tool would be at when the head 2 bit is at the 0,0 position.

When changing to a drill on either axis you may want to use another of the new features added to the VC command. Here is a sample line:

VC, , , , , , , , &On_Threshold, &Off_Threshold, Z, &DrillSW

This added command allows those with PRS drills and smaller compressors to cycle the drill motor on and off as the axis plunges. It will also allow owners of PRT drills to get functionality, but without the depth control available with a piggyback drill setup such as the PRS Drill.

The “On_Threshold” is the Z height at which the selected output is triggered on during a plunge. The “Off_Threshold” is the height that it turns off on retract. Your safe Z and rapid transit Z heights must both be higher than this number to insure proper use. The “Z” parameter is the axis that is going to do the plunge. Due to axis swap, this will always be the Z in toolchanger files. The last parameter “DrillSW” is the number of the output that gets triggered by this command. PRT drill users will need to set an offset for the Z that insures the bit will not hit the material when it plunges to the drilling depth. This is necessary to trigger the drill output. Most of the other code lines allow manual bit changes and rezeroing of the changed bits. A tool number and a C9 are called at the beginning of each file. A C7, a tool number, a C9 and then a C6 will be called up between each cutting segment when a different bit is required.

Custom6:

 The Custom6 file is used to turn on spindles, routers, vacuum, dust collection or plunge a drill used in the next cutting segment with the selected tool. IF you have these items, you should be familiar with how to enter them in a file. Another option with the SB Link is to add operations particular to a sheet, such as vacuum, to the “HEADER OPTIONS”. This way the vacuum can be turned on for every sheet and turned off at the end of cutting. Whatever you turn on in the Header, remember to turn off in the “FOOTER”. C6 will be called up after every C9.

Custom7:

 The Custom7 is used to reset all the axes to their defaults, reset offsets and settings that were added in the C9 back to those of the primary cutting head (Z). It will also turn off any outputs turned on for spindles, routers, drills or accessories. It will always be called before a C9 except at the file beginning, as nothing has been turned on yet. It is also always called up at file end.

There are specific orders in which these commands need to be used so that they work properly. If modifying toolchanger files make sure you test them to insure predictable results. You can most likely change the parameters, but be careful when changing the order within the toolchanger files. A special thanks to the ShopBot Beta Team for the lessons.

Other Useful Custom Files:

 Another option we will have when using the link will be to have a “custom file” called just before and right after an individual sheet is cut. These are setup using the sections “Header” and “Footer” in the SB Link “Setup”. Due to limitations on what can be entered in these areas, I have been using a Custom Cut callup. This allows me to enter whatever I wish to either the header and footer spots in the cutting file. Jogging the gantry to an out of the way area of the table to allow sheet loading will be the most common of these entries. Another would be to switch on or off vacuum hold down. Any legitimate ShopBot programming command can be entered into these files. Remember that these are best used for sheet specific commands, not those needed for a tool or complete cutting file (job).

Since the “Header” file is called after the load sheet message box and acceptance, this is perfect for Switching on Vacuum. You shouldn’t need to have the “Park” move in the header as it is assumed that the gantry will be parked in an out of the way location prior to starting the link.

The “Footer” file would be where you turn off the vacuum and then move your gantry to its park location. The gantry will remain “parked” thru the sheet change, and then the Header file will turn on vacuum to enable cutting the next sheet.

FlipOps:

 With the ShopBot Link we also have the option for two sided machining. These are referred to as “flip operations” in the Link. These “FlipOps” are by default done by flipping the part, oriented as it was cut, in the X direction and placing the proper corner in the 0,0 location on the table. The FlipOp beginning segment will allow you to enter an offset, in case your indexed location is not at exactly 0,0, switch an output to raise pop up pins, turn on vacuum, retract the pins and press enter when complete. The end segment will disable all of these at the end of the FlipOp and allow you to process another part.

Next month: Setup and Tool parameters.

The eCabinets design software was designed for use on only Thermwood branded CNC cutting machines. As this would apply to their CNC flatbed routers, which are single head machines with automatic toolchangers that allow bit changes within a cutting file to increase speed and expand cutting capability with the use of special purpose bits, it would also not apply to the majority of ShopBots in use today. Most of the ShopBot machines have a single head, with a single cutting bit. A small number have a second cutting head and/or drills attached to increase capability. ShopBots with automatic toolchangers are extremely rare. Most of these have been custom built for commercial applications. There has also been a recent announcement by ShopBot that they now have an Automatic Toolchanger as an option to their PRSalpha line of products.

For those of us that are not going to call and order an ATC from ShopBot to bolt on our machines, how is it that we take code that is designed for the multi bit “Big Iron” and get it to work on our smaller, sometimes self modified, ShopBots? One of the solutions lies within the advanced toolpath engine inside the ShopBot Link itself. You will be able to set cutting, routing and drilling parameters that match both your machines cutting and hold down capabilities. Once set, these parameters will allow you to add tabs, onion skin, multiple passes, reduced last pass cutting speeds, or whatever is needed, simply by entering part size parameters. For example, you can set a narrow width of 3 or 4 inches and assign tabs and/or reduced speed for the final pass. There are many more options that will allow you to cut better parts with less waste than previously possible with the vector based CAD/CAM software that has been our standard.

Another solution lies within a group of Custom Cut files that has been reserved for a toolchanger. These are the Custom6, Custom7 and Custom9. Most of us without a toolchanger have already found a perfectly good use for these files as easy access to often used cutting files. If you use, or plan to use the ShopBot Link to process eCabinets designed files, and unless you have a single axis machine, you will need to add some specific content to your Custom6, Custom7 and Custom9 files. These are the files called up in a toolchange routine by most post processors and now, more specifically, by the ShopBot Link, as it progresses thru various segments of the cutting file. If you have a single axis machine, with no attachments such as a drill, you will have to enter the text “END” in each of these files and not use them for anything else if the SB Link is to operate properly. Sorry, your favorite C#, just like mine, has to be renumbered.

If you have a single axis machine, you should plan on this when designing your files. Design around your preferred bit. Most likely this will be either a 5mm or ¼” compression bit. This bit size will be determined by the smallest hole that you have to drill in your files. If you wish to take full advantage of the hardware drilling and positional accuracy of CNC then 5mm will be the bit of choice. You should then design your dados smaller, use mortise and tenon systems or use a design that lowers the number of large dados which will eat up machining time. Process your 35mm hinge holes on a press, as these do not machine quickly with a small bit.

If you have multiple cutting heads as I do, then we need to find a way to enter all the differences in both location and operational control, and trick the SB Link output into thinking we have a single tool with multiple bits, instead of multiple heads that may be in as many as 6 different locations. Each of these tools could be called up a dozen times each in a multi sheet cutting job. This is where the 3 “custom” files come into play. In general terms, the 3 files serve the following purposes:

Custom6: This file starts your spindle or router if it is being used for the current cutting segment. It will also switch on any outputs you require for vacuum, dust collection, etc. It is always called up after a C9

Custom7: This file turns off outputs, spindles and routers, retracts plunged drills, and resets any offset required for other heads back to that of the primary cutting axis. This file is called up before any toolchange and at the end of a file.

Custom9: This file, which was originally designed to drop off and pick up bits from a tool rack, will now have the job of tricking the SB Link into thinking it is dealing with a single axis machine. Luckily for us, ShopBot is implementing a few new commands into the SB3 software and adding some new parameters to some old familiar ones. These new additions will make this “trickery” much easier. If we have added heads to our machines, the control software knows where all the additional tools are located. SB3 stores these distances, called offsets, in the my_variables.sbc file. Every offset for every tool is stored with a specific name describing what it does. These offsets will be used to offset the primary cutting axis instead of being added or subtracted to a position as we have been used to in traditional output from CAD/CAM post processors. With traditional CAD/CAM we selected a proper post processor that added the offset to the required position. When using the ShopBot Link we will have single axis commands coming into SB3 and no option to select a different post processor. Hopefully this article will give you an idea of what we need to do. As many of our machines are configured differently, we may all have a slightly different version, making these truly custom cut files.

The Thermwood tech team has been kind enough to decrypt some of the files I have processed thru the Link. In typical cutting file format, here is what happens in one of these files.

1)FILE START Link asks for wasteboard thickness. (most of us will not use this, and may not come up if it has been set to zero in settings)

2) Link asks for a sheet number or accept sheet 1 to start Link outputs “(Locate 3/4 Generic then click OK to start operation” as message box we are used to (this will be the name of the material used in the cabinet design)

3) Callup C#,90 (my_variables file)

4) Link outputs “&ZSHIFT” variable as exact material thickness (this allows us to zero 1 time to spoilboard and cut any thickness material accurately

5) C7 (makes sure spindles are off, offsets are reset, and axes are at default)

6) &tool = *** (this is the next tool needed for cutting)

7) C9 (here is where, using the tool#, we swap axes Z & A if needed, apply any offsets required, plunge a drill, select the proper output switch to on etc.)

8) C6 starts spindle, or router and switches on any required outputs

9) …(Lines of cutting code here)…

When cutting segment with this tool is complete:

C7 AND REPEAT as needed.

This will happen for every tool that is required for each sheet and for as many sheets as have been selected for cutting. Those of us that are testing the ShopBot Link for Thermwood and ShopBot are building and testing these routines on our machines. They seem to work very well. Each “Virtual Toolchange” goes by in a few seconds, much faster than an ATC could change a cutting tool. We seem to be in agreement that the ShopBot Link will be a tool that we will not want to be without.

Next Month: What is actually in the files and how to customize them to your own preferences.

The typical screw pocket is 1.5” long, 10mm wide and a little over 10mm deep. Many of the cabinet cutting and nesting software programs simply plunge the bit to cutting depth and move in the required direction, which results in a square, rather than tapered bottom. You could add these to your cabinet drawing files as a 1.5” long vector or rectangle that you toolpath to the required depth. After cutting a job using this method I decided to find a way to cut the tapered bottom pockets. There are also ways that you can “trick” the 2.5D design software to cut the tapered bottoms. You could also edit the parts file to a 3 axis move. Since I am working towards a goal of not drawing any rectangular cabinet components prior to cutting, this pocket hole cutting module will be a step towards that goal.

I have found that for my use, a 3/8” mortise compression bit works best for pocket holes. I wrote a part file that uses inputs for setting the bit diameter, panel length, width and thickness, along with the number of pockets and distance from the edge. It will cut tapered depth screw pockets and cut the panel to size (if you wish) without drawing. This allows us to cut our components with only a few seconds of machine down time. The following illustration shows a 24” by 15” panel in preview mode with 10 pockets and an outside profile cut:

Here is a picture of the mdf panel just after cutting:

 A close up of the angled pockets:

How to Use this File: (download the zipped file here)

Note: Bit must be zeroed to the top of material prior to running this file.

To cut pockets only in a panel of known size, set the panel at the 0,0 position and run the file. You will need to fill in the required inputs to complete the cutting operations. If this is the primary way you intend to make use of the file, you may want to modify the file and remove the bit diameter and trim to size options. This will decrease both cutting time and “clunky” menu lines.

To cut pockets and then trim to size, set an oversized piece of material a small distance to the negative in both X and Y. Fill in the inputs and you will have a pocketed and cut to size panel.

Another option is to use the fill in sheet and run the file in 2D offset mode. This will allow you to cut a group of pockets anywhere on a sheet or panel.

If you are drawing your cabinet parts using V Carve Pro or Parts Works you can add tapered pockets to your drawings by the following method. Unless you modify the file to fit each panel size, you will still have to enter the input lines for each size. The file will pause to allow this.

1) Draw your cabinet part as usual.

2) Place a small circle centered on the lower left corner of the part.

3) Select the circle and toolpath it using a drilling toolpath.

4) Save that toolpath using the “ShopBot Drill” postprocessor. Set the tool number to “2”

Note: you must make sure that the X & YindrillOffset variables are set to 0 (zero)

5) Open C:\SbParts\Custom. Save a copy of the “Custom8.sbc” file as Custom8.OEM (or any other name) for a backup. Open your editor to a new file and enter this line:

FP, (NAME OF THIS FILE).sbp, 1, 1, 1, 1, 2, -0.00, 0, 0, 1, 1

Save the file as Custom8.sbc in the default location.

6) This file will now run in 2D offset mode in every location that you placed a circle.

7) I would recommend commenting out the bit diameter and trim to size input lines prior to using this in the Custom8 file. This will allow you to toolpath your part cutout with VCPro/PWks in your normal fashion.

As with all untested parts files, you should air cut with it before running with a cutting tool. If you use the trim to size option, the machine will cut the panel at 2ips full depth 1 pass. You may have to adjust the cutting speeds and depth per pass to fit your machines cutting abilities. In any event, if you don’t feel comfortable modifying a parts file, this may not be for you. If you have a PRT drill installed on your machine, you will need to select another custom file number and modify the post processor to reflect that number change.

A few notes on the ShopBot Drill post processor. For those that don’t wish to hand code master files full of 2D offset subfiles, this may be one of the most versatile tools you can use. Vectric has graciously allowed us to modify (at our own risk) our ShopBot post processors. The Vectric ShopBot Drill post processor (used to operate the air drill on a PRT) can be used within a VCPro or PWks drawing file to travel the machine to a specific location (center of a circle) and call up and run a custom cut file. Make sure that you use the 2d offset parameters as shown above. To benefit from multiple custom callups, you will have to build a postP for each one. David Buchsbaum explains this in his column: http://www.shopbottools.com/notes_from_the_sandbox.htm#Customizing

If you have a machining file that you use fairly often, whether it is a special part, RTA fittings as David does, cabinet hinges, drawer slides, hanging slots, a speaker hole with mounting recess, or any other operation that you do repetitively, instead of drawing or copying and pasting in parts, consider just setting a circle on the drawing and use a modified postP and Custom cut file to do the job. You will, of course, have to make a part file that assumes a 0,0 start, cuts your part and retracts the tool before you can use it in 2D offset from a custom cut file.