Zenbot quick start notes

[rich909]

As a new Zenbot user who is also new to CNC and mach 3, I thought there should be a thread to archive discoveries, set-up, and configuration details specific to these machines. In theory, an archive of issues that we have worked through like fixture ideas, table sizing/offsets, tool feed/speed, kernel speed, who knows what else ...may become a valuable resource to Zenbot users over time.

Right now, I've got a couple of things to contribute, and by next month I will have forgotten what they are. The time to post them is when they are fresh! I believe each reply to this thread will allow a new "title" for a topic not already covered. Discussions and refinements that follow can reference that title, providing a little bit of organization.

I hope as others have insights they will contribute ideas here, and perhaps reference other related threads.

--Rich

[rich909]

When performing the first "actual" cuts on my new 12x16 running Mach-3, I saw that the Z-axis was loosing steps. The X & Y axes appeared to be ok. Initially I wasn't sure if I was making too heavy a cut causing the problem, so I tried some adjustments, but the problem remained. At that point I went back through the configuration steps starting with Ports/Pins. At the bottom of that dialog, I noticed that the Kernel Speed was set to 45,000HZ.

In the few days of waiting after I ordered my Zenbot until it arrived, I had installed Mach-3, run the Driver Test program and found that my PC (although 25, 35 & 45,000HZ all tested at 'excellent' level) seemed to work best at 25000HZ, and set it for that. How did it get changed? I set the Kernel Speed back at 25,000HZ, and re-tested the driver, which confirmed the most stable operation at the 25 speed. After that, I re-ran my cuts and confirmed that steps were no longer being lost.

By experimentation I discovered that the Kernel Speed selected from the Ports/Pins dialog is SAVED in the machine configuration file, specifically zenbot.xml. What happened was that Shaun sent me a new copy of the configuration file when he shipped the Zenbot, which I used during my subsequent tests and configuration settings. It's not his fault! He was doing me a favor in providing the "latest" version. Anyhow, I didn't notice the speed change and didn't realize that the "Driver Test" needed to be re-run to keep things in sync.

My controler PC is a 2.00GHZ Intel Celeron, with 1GB RAM, Matrox 32MB video, running Win-2k. It may be that it "will" run without loosing steps set to 45,000HZ, if I simply set it to that and re-run the Driver Test program at that speed. For now, the Zenbot is working smoothly and reliably ...and I am having too much fun to experiment with it more right now. I'll be posting some photos of the first successful projects later on.

Anyone with with additional information or insight on this topic, I hope you will share your thoughts.

--Rich

[rich909]

Because the Zenbot does not come with Home/Limit switches, it is a good idea to set up work so that you have plenty of space before the limits of motion are reached. That way you will have some reaction time if things don't go as expected.

If you are using Mach-3, the table size is set through the Homimg/Limits configuration dialog. At the start of each job, I make it a habit to load the tool path/G-Code and then go to the 'Tool Path” screen view and check the right-most panel: the 'Program Limits' display. Note the maximum & minimums for each axis, which must be smaller than the 'physical table' size of your Zenbot. With these values it is easy to set a 'Logical Table' by selecting the top line menu 'Config' and choosing 'Homing/Limits' and entering the max/min values noted earlier. The 'logical table' can be changed for each differently sized job as needed. Once the table is established you can set the 'Soft Limits' button to 'ON' at the 'Program Run' screen, you will not be able to jog/move any axis beyond the limits you have defined for the job.

After setting the 'Logical Table' jog the x, y, z axis to the desired 'zero/home' position for your work piece. Normally, this is based on the origin chosen in the CAD/CAM package used to create the tool path for the job. Once the axes are at the 'origin' change to the 'Offsets' screen view and press the 'Ref All Home” button in the right-most panel – above the 'Machine Coordinates' button. Verify that the 'work offsets', 'machine coordinates' and work DRO's are now all zero for each axis.

Creating a job-sized 'Logical Table' eliminates the need to set up a separately 'offset work table'. On a small physical table machine, it seems unlikely that you will want to keep multiple fixtures set up, diminishing the value of work offsets. Another advantage of this practice is that the the 'tool path display' will be more suitably sized without having to repeatedly zoom in. The default home/limits settings in my initial zenbot.xml configuration were +100in x -100in (about 16ft sq), which caused a minuscule tool path representation of a job and provided no protection against a crash at the physical limits.

For reference, the Mach-3 Tutorial video on Homing/Limits assumes a router/mill with home/limit switches. It takes a while of thinking about this, to realize that in a system without these switches, a table should be set up differently ...actually like work offset rather than physical table. As a consequence it is not too helpful when getting started with Zenbot or other router/mill without switches. You should note that ArtSoft recommends that Mach-3 be restarted after making changes to the configuration settings. I have not found this to be needed with table size changes, but I verify the limits of motion before the first run at new settings. To prevent possible problems it wouldn't be much inconvenience to practice the restart rule before the initial run at new settings.

These are my discoveries of a technique that works for me. If you have additional observations, questions or insights, please feel free to offer them.

[rich909]

To prevent damage to the Zenbot's table, a spoil board is recommended. I made mine out of a suitably sized 3/4 sheet of MDF. By routing a 1/2 inch wide by 3/8 inch deep slot the board can be mounted by bolts placed at the outside edges, with the heads below the board surface using the outermost rows of inserts. To provide access to the standard hold-down inserts that are now covered by the spoil board, I drilled 13/32 (1/2in ok) holes in a 2.25 matrix to allow bolts to pass through the spoil board and attach in the standard inserts. The “loose fit” allows adjustment to square the board with the table. Using 2-inch 1/4-20 bolts that have at least 1.25 inches of thread, pass through hold-down blocks, through the spoil board and into the table insert.

I made my spoil board for a 12x16 longer than the actual table which allows support of long material, that exceeds the motion limits of the machine. It is 11 inches wide and 24 inches long. You will want to adjust the size to suit your Zenbot.

The images attached show a CAD representation of my spoil board and a photo of the actual board with a fixture attached.

[rich909]

When the power to the Zenbot's driver box is shut off, the Z axis will drop to the lowest limit of travel, which is about 3/4 inch above the table . Unless you make it a habit to remove the current tool before powering down, this may result in landing the tool on the table, spoil board, or perhaps a fixture.

I've have been making it a habit to “park” my machine before powering it off. This has made it easier to set up the home for each axis at the next session. Additionally, placing it in a “safe” position at the end of the session also minimizes having to drag the axes by hand between sessions, and eliminates “landing” the tool. The practice I follow is to 1) "park" the spindle, 2) then turn the driver box power off, 3) then exit Mach-3. I use the equivalent procedure in reverse at the start of a session. That way, Mach-3 is always in control when the driver box is powered-up.

The attached photos show my swing down 'docking platform' mounted at the front-most insert on the table. It uses a scrap of plywood and a small piece of 1x1" angle iron to hold the router at a comfortable height to allow changing tools ...and provides access to hold-downs and fixtures between sessions. Being at the end of the spoil board it is safely out of the way when the machine is in operation.

[rich909]

To make set-ups easier for some of the common jobs I do, I made a couple of fixtures.

The smaller one (shown here) is for 5.5 x 6” blanks and has a fixed right-front stop with two sliding blocks to secure the job. The base of the fixture is 1/8” MDF which the front stops are attached to. It is drilled oversize holes to match a couple of hold downs (through the spoil-board) and to allow squaring adjustments to be made. The sliding blocks were cut from scrap plywood and allow about 1” of adjustment. Two deck screws in each sliding block can provide fine clamping adjustment to hold the piece securely.

The larger fixture (not shown) allows for blanks 7x13” or longer. Learning from the lessons on the smaller fixture, I cut the sliding blocks out of MDF and allowed for 3” adjustment slots. This lets the blocks adjust beyond the 2.25” between hold-down spacing. I use this sliding block to clamp the height, but use a small C-Clamp and loose spacers to secure the length. The C-Clamp is outside of the physical table, safely out of way of the gantry, ...possible because the spoil-board (24” long) is longer than the 16” table.

Included photos show the small fixture base, and the base with the two 1" adjustable sliding blocks. This small fixture is also shown with an MDF blank mounted. A CAD representation of the 3" adjustment sliding block is also included. It is based on a 3/4" MDF block, which is about 6"x3.75". The "stepped" block can be rotated 180-deg. for clamping thinner material than 3/4", when appropriate.

NOTE: Hold Down Bolts

Be careful when using 1/4-20 bolts to hold work down. Excessively long bolts can extend through the table and interfere with Y-axis movement. When trying a new fixture or clamping technique check under the table to assure the gantry won't strike any attachment points, due to an overly long bolt.

[rich909]

Just starting out with Zenbot CNC, researching and selecting a basic set of tool bits from among those available seems daunting. I had a selection of general purpose router bits already, but quickly found I needed carbide bits after I soon wore out my 1/4” shanked 1/2” 90-degree v-bit. I am still using the standard HSS bits for pocketing jobs in soft woods while I build my collection of bits.

The selections I have made so far, work for me. I hope others who have found specific tools they like ...will also contribute to this thread, so it can be a guide for those starting out.

I found selecting tool bits for use with a Zenbot depends on the spindle you are using, the type of material to be cut and the software you will be using. I'm using a Bosch Colt as the spindle. It comes with a 1/4” collet. However, to be able use bits with a 1/8” shank I needed a 1/8” collet which I purchased from Precisebits.com, along with a couple of 1/8” shank 60-deg & 90-deg v-bits.

Because the Zenbot has only 4” of Z-travel, I made it a point to select bits that were 2” or under in overall length (OAL), although bits up to 2.5” may also be ok. In the Colt, a 2.5” bit when bottomed will leave about 1.5” exposed. With a spoil board and a safe Z, you may loose 1” or more in travel, so that longer bits may limit the thickness of stock you can work with. For thin materials like 1/16 Color Core or engraving stock up to 1/8” a bit could be up to 3” long, if a shorter version can't be found.

Since I am using Vectric's V-Carve Pro as my CAD software, I followed recommendations found at the v-carve forum and purchased the Rockler Sign Makers bit set (see: rockler.com) as basic 3-bit set. These carbide-edged bits have an OAL of 2” or less and 1/4” shanks. Rockler has a good variety of carbide edged and full carbide router bits that may suit some projects.

In addition, I bought some color-core engraving bits from Centurion (see: centuriontools.com) which have a 2.5 overall length and I plan to buy full carbide 2” V-carve bits from them in the near future.

I also bought a 1/4" shank drag knife from Widgetworks (see: widgetworksunlimited.com) which is only 2.25” long and it works well with the Zenbot. So far, I have only used it to cut a few vinyl stickers, but I plan to use it on some other thin materials.

One other source of bits I've been investigating is bitsbits.com, but I haven't made any purchases from them yet.

[rich909]

Based on my experiences with the small fixture I made originally, I have re-worked a larger fixture so that it can handle a wider range of jobs, replacing the small version.

It uses an 11” x 16” piece of 1/8” MDF with 1/2” by 1/8” high moldings set at right angles on the front. The width of the work is secured by the 3” sliding block described in the original post. The length of the work is secured by an assortment of MDF blocks, which allow for adjustment, all secured by a C-clamp at the end of the spoil board. The block assortment keeps the clamp out of the range of motion for the gantry. I have attached a CAD representation of the new version of the large fixture.

The photos show the first version large fixture as seen at the rear of the spoil-board with the c-clamp securing the length of the current job. The front view shows a block secured in the large fixture.

[mactec54]

rich909

A good write up on Mach settings, one problem, I don't know how you are using the softlimits as they will not work without first homing each axes, so you need to have a home/limit switch to make the softlimits active

[rich909]

Hi Mactec54 --

rich909

A good write up on Mach settings, one problem, I don't know how you are using the softlimits as they will not work without first homing each axes, so you need to have a home/limit switch to make the softlimits active

Thanks for your input. I probably didn't explain the idea on my use of "soft limits" very well. As a relative beginner, I am hardly an expert, but let me give an example of how I use them which I discovered by experimentation.

I have a small job that requires a work table size as follows:

x= 0 to +3.5
y= 0 to +3.75
z= -0.125 to +1

...so I set the homing/limits configuration as follows

X: Soft Max=3.50, Soft Min=0
Y: Soft Max=3.75, Soft Min=0
Z: Soft Max=1, Soft Min= -0.125

After saving the homing limits for the work table size, I set each axis to where I want zero positioned on my work piece, and press the “Ref All Home” button on the Offsets screen. This of course makes the work DRO's and Machine Coordinates equal. The work table is now quite a bit smaller and inside of the 12" x 16" physical table.

With “soft limits” from the “Program Run” screen set to OFF, when I go to the MDI screen and input a command like: g0 y4 ...the Y-Axis will move to a position +4” from where I set zero and the DRO will display +4.0000. After returning Y to a position inside the work table (say 3”) and turning the “soft limits” ON and repeating the command the Y-Axis will only move to 3.75” and stop. The DRO will display +3.7500

Similarly, with “soft limits” ON ...I am not able to Jog beyond the work table defined in the Homing/Limits configuration. Yet, if I turn the “soft limits” OFF then I can jog beyond the boundaries of the work table definition. The effect is the same on any of the axes.

This whole idea has become less important to me since I have gotten more familiar with my Zenbot. Initially it seemed like a good safeguard against entering a value that would carry the controlled point outside of the area I wanted to work in. However, by toggling the “soft limits” on/off I could override it when or if needed. Now that I am more confident, I sometimes take a few shortcuts.

The method assumes that you define the work table within the limits of motion of the physical table. If not, the method will not protect you against a physical crash caused by trying to move a work table axis beyond the physical limit, as true “limit switches” would.

Incidentally, I discovered that if the controlled point is outside of the work table area, you can't turn “soft limits” on until you bring it back inside, which makes sense.

I value your feedback and suggestions, so please let me know if I am missing something here so it can be corrected.

Thanks.

--Rich

[mactec54]

rich909

So you are homing the machine,Without switches, By setting the home, somewere in the work envelope of the machine, by doing this then the soft-limits will be active as you have set & saved were home is for each axes, A different aproach but nothing beats having a proximity or switches for homing

[rich909]

I ordered a spring loaded diamond drag bit from bdtools on ebay. It is made out of stainless steel, is reasonably priced and included free shipping to continental US addresses. It arrived this past Saturday so I was able to give it a try over the weekend. It worked great.

Like the default Diamond Drag tool in the V-Carve tool database, the tool has a 1/4" shank, 90-Degree .02 tip on the replaceable .125 diamond bit. Based on vendor recommendations I used a feed rate of 15 IPM and plunge of 5. I kept the pressure at the .03 used by the default tool “Quick Engrave” tool path and set the Z-Axis zero on the loose side.

My test usage was a small job (1”x4” plant label for a friend) but it engraved uniformly across the work. I've included a couple of photos and included some details of the jig I made to do these in the future. The jig has parallel cuts that give a snug fit for the 1” aluminium c-channel. They also support it providing a level engraving surface. It is cut exactly 4” so that if fits snugly between two spacers that trap the channel preventing lateral movement. A tight press fit allows a finished piece to be popped out and a new one popped in without having to change the clamping.

I think the pressure may have been a bit more than actually needed so for the next job I will try it with 0.0278 - 0.0250 pressure or so, which I think will work as well, and still not give “light” areas. Anyone else with experience using this tool, please feel free to contribute your own experiences and discoveries.