Will a ShopBot run files with multiple bit sizes in one file?

[amy_brown]

Somewhere on this board I saw a statement about the ShopBot not having the ability to have different size tools in one file. Is that true? With MultiCam we set all our bits in one file and it would stop when we needed to change bits. Does this not happen with ShopBots? That's very strange to me. So no matter how many thousands of dollars you spend on software you would still have to do different files for every tool?? Please enlighten me.

[Brady Watson]

Amy,
Sorta...While your design and toolpath info will remain the same, you would choose a different post-processor for the ShopBot than the Multicam. You simply select the appropriate post in your toolpathing program and save the file.

Now, if you are creating a toolpath that requires 2 or more tools, then you just save each toolpath as a seperate file. This way, when the file is complete you turn off the router, tool up and call the next file to run. I think that this is much safer than grouping the files together.

It IS possible to group both toolpaths in one file with a pause command between them to change your bit. However, this is more work and there is no apparent advantage to doing this.

-Brady

[David Petrie (Unregistered Guest)]

Brady,

If you had a second Z Axis could this simulate a tool change?

I am newbie to Shopbot and I appologise if this has been discussed before.

[kerrazy]

I'll field that one Brady,
A second Z will only work in this situation, if you edit your file to include an offset for the second Z. As both tools can not be in the exact same spot due to their configurations on the Y car.
If for example you were to hog out the background of an item with a quarter inch bit and use the same quater inch bit to cut the profile of the object, you could do that process in one file, ensuring your cutting order does the hog and then the profile pass.

As for Amy's question, you could include a statement in your file or set up your software that will allow tool changes on the fly. The problem is you would also have to remember to include a zeroing routine for each bit being used.

I usually group all my similar cutter files together and then save them as one file so if there is a problem, I can just run that one file rather than rerunning the entire batch of files.
Dale

[amy_brown]

So if I have a file and it has an offset cut with a 1/4" bit and a 90 deg. v bit all in the file, I will need to save two different files and start each file individually? Is that correct.

Sorry for dumb questions, I'm just accustom to MultiCam. Yes, you have to re-zero between bits. Multicam would run the one bit and then stop and ask for the next bit in one file. Even if I have twenty different tools in the file. I could pick them individually in Enroute and run just that toolpath if needed as long as the machine was still homed in the same position.

Does the ShopBot keep it's home position between bits(files) or do you have to reset that home everytime as well?

Thanks. I'm just trying to make sure I'm buying a machine that will do what I want it to do. I'm confused because it seems everything is so different from what we're used to around here.

[bill.young]

Hey,

I'm always looking for new ideas for Virtual Tools ( and ideas for the upcoming Programming Camp!) ...is there a need for a tool that makes it easier to do what Amy wants to do? Maybe a program that lets you select all the files that you want to run and that then creates a single file that calls the others in order and inserts the pauses and z-zero routines? You would still have to create the part files for each bit as a seperate file, but it would simplify running them.

Any thoughts?

Bill

[kerrazy]

Hey Amy,
it will keep its home position, and you could do what you are trying to do, that option is all in the software you choose.
Dale

[kerrazy]

Bill,
As Amy suggests, Enroute does it automatically, and I am sure you can set it up in profileLab as well.
there is a spot to edit the commands in profileLab, where you could automatically insert commands to activate additional files or routines at the beginning or end of a file, such as the SO command.

[richards]

Amy,

Bit changes are a piece of cake. I ran some parts that required several bit changes. The process was very simple.

1. In PartWizard, I created a tool path for each operation to be performed - you may prefer something other than PartWizard. I use it because it works for me.

2. I inserted the first bit (5mm to drill shelf pin holes), zeroed the bit height using Shopbot's Z-Zero tool and software (be sure to buy or make a Z-Zeroing tool), and then ran the file that contained all of the holes to be drilled by the 5mm bit.

3. I inserted the second bit (3/8-inch spiral downcut) to do the rest of the cutting, zeroed the bit with the Z-Zero tool and software, and then ran the file containing all of the holes to be drilled with the 3/8-inch bit.

4. With the 3/8-inch bit still inserted, I ran the file to mill out an area for each of the bolt heads.

5. Again, with the 3/8-inch bit inserted, I ran the file to cut the rabbets and dados in all of the panels.

6. Finally, again with the 3/8-inch bit inserted, I ran the file to cut the perimeter of each part.

Total time to cut all of the parts to make a computer cabinet was just over five minutes (using a PorterCable 7518 router, which required several perimeter passes at 16,000 rpm to cut the part).

Later in the day, I used DoorBot to cut some doors, which required four bit changes. Using nearly the same proceedure, I had six doors routed in less than 1/2 hour. Not bad for a newbie that has used the Alpha for just a few days.

What I have learned is that I can work much faster if I create each part separately in AutoCad Lite, create the tool path files using PartWizard, and then create a master parts-nesting layout drawing in AutoCad prior to writing a master file that links the tool-path files using the J2, X, Y command followed by the FP, file-name,,,,,2 command (please check the command's syntax-I'm writing this on a computer that doesn't have Shopbot software installed). The J2 command positions the router at the starting point for each piece and the FP,file-name,,,,,2 command uses the position generated by the J2 command as a X-Y offset.

[bleeth]

The difficulties will start to show up when you want to do something like hog out an area with a larger bit and then get into the tight areas with a smaller bit. I learned the hard way that the z-zero plate is not that precise and after area clearing with a half inch endmill and going in with a smaller bit to clean out the tight areas when my project was done the half inch bit and the eighth cut at two different heights. If anyone knows a way to cure this short of trial and error or a "test" field I'm all ears.

Dave

[amy_brown]

Thanks everyone.

Dave, do you always run the zeroing routine in the same place? I saw that with MultiCam as well. Don't think it was the router but rather the fact that the material wasn't level across the table. We didn't have a vacuum pump.

[amy_brown]

Michael, where do you get DoorBot?

[beacon14]

Dave,

Don't be so quick to fault the z-zero plate. Often, as a workpiece is routed, especially with a large area-clear, internal stresses are relieved with the loss of material from one face, and the piece moves (warps) imperceptably (to you and me, anyway). It only takes a few thousandths to notice a step at the interface of the two cutting paths. Even with a vaccuum set-up, these stresses can cause movement, and it can happen with solid wood, plywood, MDF, metals - just about any material.

You will often see a step just by going over the same toolpath with the same bit, without re-zeroing.

[fleinbach]

There are 2 other things to watch out for using the Zero plate. The first one is two make sure the plate is completly flate on the surface you are zeroing to. The spring cord on the plate can cause it to float a bit giving a false reading. Holding down the plate will make sure it is flat on the surface and give an accurate reading.

The second problem was related to how I was holding down the material. I cut mostly large panels from MDF and do not find a need for a vacum system as yet so I use a few screws to hold the sheets in place. After not cutting all the way through the sheets a few times I fianaly paid attention and found that the corner I was zeroing to was slightly off the table. I have always been impressed with how flat and stable MDF sheets where. But that is only true if they are from a new stack that has been properly stored. Once that stack is broken open and they are restacked they will take on the shape of there new support. This happens very rapidly in as little as just a day or two. So now I make sure I am holding down pressure on the spot where I am zeroing to.

[bleeth]

I do zero in the same area, make sure the plate is flat on the workpiece and use a vacuum holddown. I received an e-mail hint to go to a fixed safe z height to remove the old bit and put in the new one with a same height block as a guide, rather than re-zeroing. Sounds like a good idea.

[ron brown]

Dave,

When something is really critical, I will have a part off to the side I have cut to a known height. I will then make a pass with the "new" bit and adjust the "Z" as neecssary.

Even then, the flex of the machine and bit forces sometimes cause the cut to not be "perfect". It happened more with my old "PR?" I adapted from a cable-drive machine than does with my new machine which is a lot stiffer.

Ron

[richards]

Amy,

The DoorBot program was listed in the Forum a few months ago.

Contact:
Wes Mason
Mason's Millworks
DoorBot CNC software for Shopbotters
www.doorbot.net (http://www.doorbot.net)

I believe the cost was $250. The program is good, but there is still some handwork that you'll need to do to clean up the corners and some sanding with a profile sander.

Mike

[Kevin Reid (Unregistered Guest)]

I run multiple bit profiles almost every day. What I have done for a zero plate is mount plywood to the end of the bot at the home corner of the table and about 10" along the y axis, with an aluminum sheet on top. The whole thing is lower than my spoilboard so I wont cut it when running along the table edge. I set my zero routine so that by using this the bit is zeroed to the table height, and I just set my software for table zeroing instead of material height. Works great! And since I come home to change bits and rezero, I havent seen the need to make mulitple tools into one cut file.
Kevin Reid

[paco]

That's GREAT Kevin!

I've seen this setup on laser and such but had'nt clearly design it for my machine yet. Tell us more about the adaptations you've been througt to use spoilboard zero instead of material zero...
By the way, I've modified zZero.sbp file to use it as a material gage...

[kerrazy]

Dave,
I run into similar problems and what is truly the concern is the amount of contact surface for the smaller bits. Especially any kind of a spiral bit. If you look at the geometry of tthe bit it is in fact not flat on the surface, but it is angled, reducing the surface area of contact for the z-zero plate.
I do a lot of files where I hog out with a large bit and come in with successively smaller bits to get around letters or into corners. The secret is to put a piece of regular 8.5 X 11 paper between the material and the bit and bring the z down until it just pinches the paper. From there set your Z-Zero and you are good to go. It has never failed me yet.
Dale

[richards]

Dale,

For precise work, I use the z-zero plate and then check the height with a feeler guage, make any adjustments and start routing. It's one more step, but it takes care of the problem with a small contact area.

Mike

[daveiannone]

I have had the same problem once in a while....
I think Ron Brown's remedy (with a piece of scrap off to the side as a "test" piece)sounds like the easiest & most accurate solution to this.Thanks for the tip Ron.

Dave I