Basic Cutting Tutorial
 

This thread is designed to give the forum members, with no experience in CNC, an idea of what is required to cut out a simple design using relatively inexpensive 2 1/2D(imension) CAD and CAM software. TurboCAD Deluxe is the CAD program I use and it retails for around $100. The CAM program I use is SheetCAM and it is around $150 give or take a few $$ depending on the current exchange rate.

It is not intended to be a tutorial and I don't believe Gerald will want his forum tied up with indepth discussions about either of these software packages. Forums already exist for that purpose.

If anyone wants to add something, please feel free. Also, if I have put out incorrect information, please don't hesitate to correct me. I'm not sensitive.

OVERVIEW OF THE PROCESS:

1. Draw your object and set the correct layers (done in your CAD program).
2. Add the specifications for the raw material from which you will be cutting the object (done in your CAM program).
3. Open the drawing and specify the correct settings (feed speed, tab locations, etc.)(done in your CAM program).
4. Run the post processor and save your G Code in a tap file (done in your CAM program).
5. Open the tap file (in MACH3).
6. Zero the machine coordinates for your Mechmate (in MACH3).
7. Set the zero for your workpiece (in MACH3)
8. Cut out your object.

This is the object I will make. It is a 6 inch by 8 inch rectangle with a small circle cut out of the middle.

Attachment 5779

DRAW YOUR OBJECT

We begin in TurboCAD by selecting the "rectangle" icon.

Attachment 5780


Click the first corner where you want your rectangle to be located and drag and release the left button of your mouse when you have reached the opposite diagonal corner.

Attachment 5781

The rectangle is 6" X 8".

Next, we want to draw the circle that will be cut in the middle of the rectangle.

Click on the "circle" icon shown in the red circle.

Attachment 5782

Click on the screen at the location that you want the center of the circle to be. Drag the cursor and release the left button when the circle is the desired diameter.

You must ensure that the rectangle and the circle are in different layers. I'll explain why in the text below.

Attachment 5783

Save your work as a DXF file so that SheetCAM can use it.

Attachment 5784

ADD SPECIFICATIONS FOR YOUR RAW MATERIAL
Next, we want to open SheetCAM and create some G Code.

I wanted to show a full screen shot like I have for TurboCAD and MACH3 but for some reason, the full screenshots for SheetCAM were almost illegible so I blew up small sections of the screen where there is information that was important to highlight. No big deal because from what I remember, there is only one main screen in SheetCAM and all the settings are done on drop down menus.

This screen shows where I am setting the dimensions of my sheet of plywood. In this case, it is a 23" X 49" piece of 5/8 inch thick mdf. You can reach this drop down menu by selecting "Options -> Materials" in the menu along the top of the main screen.

NOTE: Look at the material thickness. It says .635" I'm going to discuss this number later in this thread when I get around to zeroing my Z axis.

Attachment 5785

OPEN THE DRAWING AND SPECIFY THE SETTINGS

Under the "file" selection on the menu, select "open a drawing." Find your file and select it. The drawing will appear on your material. My SheetCAM is setup so that the drawing always appears at the very bottom left of my material.

Attachment 5786

Since my clamps are positioned to hold down my sheet of plywood at the very bottom left, if I don't move the drawing, the router bit will cut into my clamp. Click on the "reposition drawing" icon and position the drawing to your satisfaction. Then click the "scroll screen with the mouse" icon when you have moved it to the proper location. If you don't click on the "scroll screen with the mouse" icon, SheetCAM won't let you do anything else.

Attachment 5787

Attachment 5788

Next we want to tell SheetCAM to cut outside of the rectangle so click on the "edit contour" icon. Since we drew the rectangle in layer 0 in TurboCAD, we have to tell SheetCAM that this outside offset applies to all objects drawn in layer 0.

Notice that at the top of this "edit contour" window there are four pages. Most of the settings on these pages are pretty much standard and once they are set, you don't mess with them much unless you change from cutting wood to cutting aluminum or styrofoam.

It is kind of hard to see but notice that both the "cut depth" and "Z increment" boxes contain the number .686" That means that I'll be making only one cutting pass. That is hard on the router's bearings so I'm only cutting at 1 inch per second. If I wanted to make two passes, I would enter something like .343" in the "Z increment" box and I could theoretically increase the feed speed.

Also, notice that the "cut depth" is .686" but my material is only .635" I'll discuss these numbers later in this thread when I zero my Z Axis.

Attachment 5790

The next screen shot shows the "cut path" page. On this page, you can set the tab length and thickness. The size shown on the screen works for me but you can easily change it.

Attachment 5789

Here, I have zoomed in on the part to show the cutting path for the outside of the rectangle. Notice that SheetCAM is telling the router to traverse from the start point at the bottom left of the material to the top right hand corner to beginning cutting. Since we are only cutting one part, it doesn't make sense to move all the way across the part to start cutting. We'll change that to a quicker start point.

Attachment 5791

Click on the "start point" icon and then click on the new starting position on the rectangle. I forgot to get a screen shot of the "start point" icon but it is the button with an "S" on it and it is located beside the "tab setting" icon.

Below, you can see that we have a new starting point.

Attachment 5792

Now, let's place some tabs to hold the work piece so our dust collector doesn't suck it up and\or the router doesn't spin it around and mangle the edge. Click on the "set tabs" icon and then click on the perimeter of the rectangle where you want to have a tab. I normally only put two tabs. The router doesn't generate that much force and two will usually hold it. One complaint I have about SheetCAM is that it doesn't provide a method for removing tabs so be careful where you put them. NOTE: If you forget to set your tabs and decide to add them later in this process, make sure that you have selected the appropriate contour or you will be driven crazy trying to figure out why SheetCAM won't let you set the tabs. In other words, if you want to set tabs for the outside offset contour, select that contour in the lower left hand box. I've accidentally done this several times and it is pretty frustrating.

Notice in the screen shot below that the tab is represented as a short blue line in the perimeter of the rectangle.

Attachment 5793

Now, we need to tell SheetCAM to cut inside the circle. Select the "edit contour" icon and...

Attachment 5794

change the layer to 1 and the "contour method" to "inside offset."

Attachment 5795

Click "OK" and the inside offset cut path will be displayed for every object that was drawn in layer 1. If we had two circles drawn in layer 1, SheetCAM would automatically calculate the best cut path for both of them. Notice that the green line is on the outside of the rectangle and on the inside of the circle.

NOTE: If you ever have trouble setting up SheetCAM so it will cut an offset, the most likely problem is that your object is open. In other words, the lines that form the perimeter of your rectangle are not completely joined. When that happens, SheetCAM sees your rectangle (or whatever) as simply a set of lines to follow so it cuts down the center of the lines rather than outside (or inside) of them. Single lines don't have an outside or inside to them!

Attachment 5796

RUN THE POST PROCESSOR AND SAVE YOUR G CODE

Next, we need to run the post processor. We are still in SheetCAM. Click on the "P" icon at the top of the screen and a drop down menu will ask you where to save the file and what you want to name it. Remember the name and where you saved it because MACH3 is going to need this file. It contains your G Code which are the instructions for cutting out your work piece.

Attachment 5797

You can also ask SheetCAM to estimate the cutting time. The "alarmclock" icon is what you would click to get your estimate. I always perform this task just to make sure that I haven't done something stupid. This cutting time looks reasonable so I've probably done everything right and I'll go ahead and proceed.

Attachment 5798

OPEN YOUR TAP FILE

Now that we have our G Code written, we need to move to MACH3. The best thing for a new CNC operator to do is to make a trial run in MACH 3 to make sure the G Code is written properly. I still consider myself a new CNC operator so I always perform this task. So far, I have wasted very little material and haven't damaged my router. Guys like Sean R and Sean D probably omit this step since they are working in a production shop and have lots of experience. I'm sure they never make mistakes either.:)

I have MACH3 installed on two computers in my house. You are allowed by ArtSoft to have up to three copies installed per each license. One copy is installed on my laptop and the other is installed on the computer which is attached to the control box for my MM. This setup allows me to do my CAD drawings and G Code development in my office and minimize garage time since it isn't as comfortable as my easy chair and I'm not a rugged bearded South African he-man.:D:D

Below is a screenshot of MACH3. I had to split it in half to get it big enough so you could read it. Once you have it set up, you really don't mess with the settings a whole lot. Maybe I should say that I don't mess with the settings much.

Select File->Load G Code. Choose the appropriate Tap file (your G Code file). When you click on your tap file, it will load into the window on the left side of the screen. As the G Code is executed by MACH3, the file will scroll by in this box.

Notice that the starting lines of your GCode file will appear in the box and a picture of your part will appear in the small screen on the right. Click on the green "Cycle Start" button and watch the small screen. MACH3 will simulate cutting your workpiece. The pink crosshairs are a "top down" view of your cutting tool and as MACH3 cuts out your part, the crosshairs will move around the drawing. Pay particular attention to the small arrow that is pointing down on the right side of your small screen. This represents your router bit. I always make sure that I see it go up and down in the location where I have placed my tabs. If you don't see that happen, you either missed it and need to watch the process all over again or you forgot to place tabs in SheetCAM. Fix it now because you will just waste wood and\or damage your dust collector foot if you don't.

Attachment 5799
Attachment 5800

Once you are sure that your G Code is properly written, you need to move to your router and set up your cut.

ZERO THE MACHINE COORDINATES

The first step is to ensure that your machine knows where the home for X,Y, and Z is. To do this, use your keyboard to move to the "zero" extremes of all three axes and press the "ref all home" button on the MACH3 screen. Ensure the "Machine Coords" icon is selected before pressing the "ref all home" icon. The frame around the "machine coordinates" button lets you know if you are looking at the "machine coordinates" or the work piece coordinates. When the button's frame is lit up in red, you are viewing the machine coordinates. When it is not red, you are viewing the "workpiece coordinates." This will make more sense as we move farther along in this tutorial.

In the picture below, you can see that all of the axes for my MM are at the home position. If you have proximity switches (I don't), your machine will automatically move to this position and it will tell itself that it is home. I have to use the keyboard to move the axes to this position and then click the "ref all home" button. Fortunately, you don't have to do this every time you use the machine. As long as you don't accidentally bump one of the axes out of position, you can shut your machine down and when you turn it back on, MACH3 already knows where the cutting tool is. All you have to do is set the workpiece zero and that's what we're going to do next.

Attachment 5801
Attachment 5802

SET THE ZERO FOR YOUR WORKPIECE

Now that MACH3 knows where "machine home" is, we need to tell it where the "workpiece home" is located. Ensure you have deselected "Machine Coords" by pressing that button again. Let me repeat it one more time, when you are setting the "Machine Coordinates" or "Machine Home" a red box will appear around that button on the MACH3 screen. When you are setting the "Workpiece Home" or "Workpiece Coordinates" the box around the "Machine Coords" will NOT be red.

This photo shows where I imagine my part will be cut out of my board.

Attachment 5803

Now, using the keyboard buttons, move the tool bit until it is directly above the bottom left corner of the location where your part will be cut out.

Attachment 5804

Here is a closer look. You can see the router bit sticking down below my dust collector foot brushes. Since both the X and Y axes are correctly located, you can tell MACH 3 that they are located at the workpiece home. Do this by clicking on the "Zero X" and "Zero Y" buttons. They should now read zero. Ensure the "Machine Coords" button is deselected before you zero these axes.

As you can see in the picture, I have a large space of plywood available and a small part so I don't have to get the cutting tool EXACTLY in the proper position in the X and Y axis. I probably played with the keyboard long enough to get within 1/2 inch in both axes. However, use commonsense. If your plywood is 49" wide and you are cutting out an object that is 48.75" wide, you are obviously going to have to be more accurate when positioning the bit or you will run off the edge of your plywood. Zeroing your Z Axis requires more accuracy but I'll get to that later in this thread.

Attachment 5818

Compare this screenshot with the screenshot above before we zero'd the workpiece. Notice how the drawing has changed positions and the X and Y locations have been zeroed.

Attachment 5805
Attachment 5806

Next, we need to Zero the Z axis. I don't know how most of the other MM owners do it but this is my system.

I first move the cutting bit over the table and then press the "page down" button on my keyboard to lower the cutting tool until it is barely above the workpiece. Below is a photo of me using a .010" feeler guage to set the height. When the bit is close enough, I press the "Zero Z" button. Again, ensure the "Machine Coords" icon is NOT selected. Now, MACH3 knows where the top surface of the plywood is and where it will start to cut out your rectangle.

[NOTE: Remember earlier when I set the material thickness at .635" and the "cut depth" at .686"? If I am able to set up the Z Axis on my Mechmate so that the bottom of the router bit is exactly even with the top of my plywood and I zero the Z Axis in that position, then my router bit will cut through the workpiece and into the spoilboard exactly .051" which is the difference between .686" and .635" For me, it has been harder to do than it sounds. You are probably thinking that all you need to do is to run the router bit down until it hits the surface of the plywood and press the "Z Home" button. The problem is that the teeth of the pinion gear on the Z Axis motor start to slip against the teeth of the Z Axis rack when the router bit is stopped by the plywood. Remember, the motor mounting brackets are spring loaded so when the bits hits the plywood and the teeth slip, the stepper motors think they are below the actual surface of the plywood. If you began your cutting right now, you would cut farther into your spoilboard than you intended. However, there is an easy solution.

I place a .010" feeler gauge between the router bit and the plywood and then drop the cutting tool down until it is somewhere near the feeler gauge. Because you know the gauge is .010" thick, it is easy to estimate whether the space between the bit and the gauge is less than .041". If there is more than .041" of space, my cutting tool won't cut into my spoilboard and the workpiece won't be completely cut out. If the cutting tool touches the gauge, I run the Z Axis back up an inch or two and then drop it again. This ensures the teeth are fully meshed.]


Attachment 5807

Now, you are ready to cut. Turn on your dust collector and press the green "cycle start" on the MACH3 screen. I still hover over one of the machine's emergency stop buttons until I'm sure everything is going as planned.

Below is a photo of the workpiece after it was cut out but still hadn't been removed from the plywood sheet. I normally use a hammer and chisel to quickly sever the tabs linking the workpiece to the sheet.

Attachment 5808

If this process seems overly complicated to you, don't worry about it. It is much easier to master than you might think and once you have all of your software packages installed and your Mechmate sitting in front of you, it will all make sense. If you are serious about building a Mechmate but can't start right now for some reason, I recommend you buy a CAD program and start playing with it at night. Creating my drawings are currently the most challenging part of this process for me.

excellent post
thanks!!

Well, you're a day late in my book. ;) since I cut my first parts today. BUT... thanks for the great tutorial, I am sure it will do many people much good. It seems like the perfect thing to give the rough run-down of the process.

AND, even though I'm a seasoned professional (with about 45 minutes of CNC operation under my belt) you just taught me about the way the zeroing system in Mach3 works, the difference between machine and part 0. I was just resetting both every time to make sure it would cut the part right, I was going to worry about machine 0 once I had my proxies installed.

Thanks for a nice addition to a great forum to learn how to use the plans and machines created by the generous Gerald and all the other contributors.

Doug, this is a fantastic introduction to the whole process! Thank you very, very much!

Thanks guys. Gerald, I'm sorry it took me so long to put this together.

I'm already finding flaws in it and missed opportunities. For example, I should have explained the relationship between cut depth, the feeler guage, and the spoilboard. But there are so many things to consider and explain, if you tried to address everything, the post would have been so large, no one would have read it.

I assure you that I did not read.
I will read it later.
But I know that work is to organize, write, cut, paste photos. (Time-Time)

THANKS DOUG!!!

Outstanding contribution. Thanks Doug!

My pleasure Ros and Jeff. Gerald was kind enough to let me edit it so I could fix my errors.

If I have confused anyone, please don't hesitate to ask a question. I'll do my best to clarify.

On using the feeler gauge for height setting, we actually use paper and take its thickness as zero. When the paper is "gripped" then hit the zero button.

Thanks Doug. I still have to learn most of this a little later down the road. It is nice to start reading the set procedure know and get use to it. It works a lot better with the older mind. :)

Thanks Doug: Very inspirational for someone just starting out on the MM trail. Nice to know there is real dust in the road ahead! and how to get it without crashing the machine!:)

Y'all are welcome. I enjoyed writing it. Good luck in the future.

Well done Doug.

The only small correction I would make is that there is only one way to zero machine coordinates. That is by referencing.


Whether or not the machine coordinates are selected, pressing "zero axis button" will not do it. It will only zero the current work coordinate.

So no need to worry about accidentally resetting machine coordinates.

As I said, good job.

Greg

Thanks Greg.

I'm not sure I follow what you're saying but I trust you. Based on the posts you made in the past, you know a thousand times more about this stuff than I do. Thanks for correcting me.

On second thought, maybe I do understand. Are you saying that if the "machine coordinates" button is accidentally selected when you zero the Z axis, your Mechmate will think that "machine zero" for the Z Axis is at that location therefore the workpiece zero for the Z Axis must also be at that same location?

I've been thinking that I could improve my tutorial by adding a brief overview (or road map) of the process at the very beginning of the first post and by adding an analogy (if Gerald will let me). At the moment, I can't really come up with a good analogy for zeroing the machine and the workpiece. Can anyone suggest a commonplace analogy I can use?

Doug

I don't want to clutter up your excellent thread.

Whether machine coordinates are being shown or not, zeroing and axis DRO by pressing the on screen button will only zero the current work coordinate.

It will not zero the machine coordinate. That can ONLY be done via "referencing / homing"

Have a play around with it and you will quickly see. :)

Greg

Greg,

I REALLY appreciate your input and now I think I understand what you've been saying. Wow! You learn something everyday.

I'm thinking I should change it to say:

The frame around the "machine coordinates" button lets you know if you are looking at the "machine coordinates" or the work piece coordinates. When the frame is lit up in red, you are viewing the machine coordinates. When it is not red, you are viewing the "workpiece coordinates."

And then elsewhere, I'll add verbiage that says something like:

The operator should move all of the axes to the home position, push the "machine coordinates" button so he can view the "machine coordinates" and press the "ref all home" button. When the DROs all read zero and the "machine coordinates" button is framed in red, he has verified that the machine is properly zero'd.

And finally, I'll write:

Press the "machine coordinates" button until the red frame is not lit. You are now viewing the workpiece coordinates....(additional verbiage here)...Press the "zero X axis" button to properly zero this axis....


If I'm on the right track, please let me know and I'll make the changes. Seriously Greg, thanks a million.

Sounds pretty good to me Doug. :)

Maybe Gerald or one of the moderators could now delete the last few posts to keep your thread clear.

Greg

I think it is good to have the interaction visible, it should encourage others to give input and let Doug refine his tutorial. Thanks everyone!

Thanks a million Gerald for being patient with me and Greg for taking the time to read this lengthy post and straighten me out.

If anyone sees any more problems, please don't hesitate to point them out so I can fix them. We owe it to those members who are new to CNC to make sure we don't mislead them.

Dough

thanks for nice post. As a supplement to your post and setting Z axis I would like to post this link:

http://www.cnczone.com/forums/showthread.php?t=56079

I bumped into this and think it is worthy to share it with fellow MM-ers.

Proper Z position
 

After reading Dougs post and listening to the Mach3 videos, I feel I have not set my MM up correctly. I have my Z axis homed to the top of the stoke at 0.00. When I lower the Z axis toward the table the DRO for the Z axis increments in negative numbers. I set this according to the Mach3 videos, but Doug seems to have his DRO numbers incrementing in positive numbers as he approaches the table. I have tried to play around with Mach3 in the homing/limits screen and reverse the DRO to positive when jogging down (using the page down key, like Doug explained), but I haven't been able to do it. Should the Z axis traveling down be giving me a positive DRO number and if so, can someone walk me through the procedure to set it up in Mach3?:(

A Z-axis going down should increment a negative number. The zero is set after every tool change. There are 2 popular points to set zero:
- the tooltip touching the table surface, or
- the tooltip touching the top of your job.

Nice tutorial for beginners. I use to use the feeler gauge method until I found this tool. Works the same way but is more repeatable and accurate. There is also wiggle room in-case you go a little to deep;) Should mention that the .0004 accuracy should be more like .001 seeing that is the smallest it can measure.

http://cgi.ebay.com/MAGNETIC-Z-AXIS-...item5193f0eef3http://www.shars.com/files/products/.../303-3104B.jpg

Excellent work. Thanks for sharing.