View Full Version : NEED HELP - Circles w/holes

08-04-2008, 02:08 PM
We are a new user & encountered a quick problem - we are trying cut shapes (12" to 26" diameters) that have a 1/2" hole cut inside of them, and cut as many as possible from a 4' x 8' sheet. If we allow the shopbot to do this, it wants to cut all the center holes first then come back and cut the outside shapes. We are finding this results in all the 'center holes' being off center by 3/8" minimum.

Any suggestions?/ideas?

08-04-2008, 03:20 PM
I believe you can change the "cut order" within the program.

Also the easiest way is to make 2 toolpaths out of this file by selecting all the big holes for one toolpath and another for the 1/2" holes. Then select the toolpath for the small holes as your first toolpath to cut.
Although I don't think that is why your cutting is off.

08-04-2008, 03:40 PM
What software are you using to create the cut files? If you can post an example of what your shape looks like and maybe the file you are using we can probably figure it out. It sounds like a toolpathing error.

08-04-2008, 04:44 PM
Jack, what is the reason you think our cutting is off? We tried the 2 toolpaths idea and that's how we ended up with the center holes so far off; David, we are using Partworks to create a 16" circle with a 1/2" hole in the center

08-04-2008, 05:29 PM
Casey: Check that your outside circles are coming out truly round. Make sure your toolpaths are created in arcs inch format. If you want one of the shapes to be cut in a different order than create different toolpaths for each one and save them to the toolpathing file in the order you want to cut.
If your circles are not coming out truly round than you have an "out of square" issue that can also result in other things (the center drilling) being out of alignment. Fine tuning for squareness of all axis' and making sure your z is perpindicular to the table is critical. If this is a used or new machine you must make sure the v-bearings are seating correctly in all positions on the tracks. If a used machine I would be checking my gantry rails to be sure they are straight and flat. Getting your machine set up for precise work usually takes a decent amount of tweaking. From the x rails being dead parallel, straight, and level to the y being dead perpincicular and also straight and level, and the z being right on 90 degrees to a well flattened table if each is off by a little you can end up with some pretty major errors.
On the design side if you are sure you created your inner circle at the center of the outer you should group them prior to moving them around for copying and nesting just to be sure you didn't accidentally move one without the other moving with it.

08-04-2008, 06:44 PM
Not knowing what pgm you used to toolpath with I was just trying to speculate on what the problem is.
Although this suggestion is a PITA it might help you figure out when/where your problem is coming in to play.
I would toolpath each hole sperately for one 4x8 piece of plywood and try it, cutting one at a time and checking each one.
Maybe a picture or 2 might help us visualize the problem or recognize whats going on. Maybe a cut file for us to load up to see what its doing in preview.
Since you seem to be a new user it is probably a "rookie mistake" that we can recognize (since we all still make them from time to time).

08-04-2008, 06:51 PM
It's possible you have a very small vector that's an unwanted separate piece that will throw off the ability to center or do other functions.

To be sure- "select all" and group. Then you can double check to see that the only two vectors are the inner and outer circles.

08-04-2008, 06:53 PM
You have a nice operation, going there.

08-04-2008, 09:22 PM

I would check two things in Partworks. First, make sure you have setup the software to machine inside the circle instead of outside or on the line. Second, check that you are using the same diameter tool that you selected in Partsworks.


08-05-2008, 03:22 PM
Is it uniformly off center on every circle? Is it good for the first couple then gradually gets off center?

If you are cutting too fast and lose steps you can end up w/ results like what you describe.

Basically it does what you tell it to, can you post your cut files?

08-05-2008, 06:27 PM
Just out of curiosity, how do you know if you are loosing steps??

08-05-2008, 10:20 PM
Things happen like 1/2" holes that should be perfectly centered are not...

08-06-2008, 09:56 AM
If the ShopBot thinks it's in one place but is actually in another place...you might just have lost a few steps..

08-06-2008, 10:50 AM
An easy test to find the maximum feed speed that you can use with a particular cutter and a particular type of material before "losing steps" is to cut a series of straight lines, each starting a the "0" end of the material. Start with a moderate speed, maybe 2" per second, and then progressively cut faster. Look at the start point and the end point on each 'line'. When a line is shorter than its neighbor, you've begun to lose steps.

If you're critical you'll cut some lines along the X-axis, some lines along the Y-axis, and some lines 45-degrees diagonal between both the X and Y axes.

08-07-2008, 12:44 AM
what size of a bit are you using? I goofed today and did a pocket of a .375 hole with a .375 bit and ended up with a oval. I caught it and changed it to a drilling toolpath and no more problems. so if your using a 1/2" bit this could be an issue.

08-07-2008, 08:00 AM
I like to drill a "registration" hole in my work. Since I don't use vacuum, I cut this when I cut my holddown mounting holes. I like to put it in a corner, and sometime I put down several. Also its nice to make the coordinates of this hole some nice round number like (-6", -6"). This way, if you lose steps, or suspect it, you can move back to this hole and find out if you are off from it. If you are, you can recenter to this hole, and like the example above, zero to the hole, m2 6,6 which will put you back at the original center and "z2". It also helps something goes wrong, you can get back to your original coordinates referenced to your workpiece.

08-07-2008, 09:43 AM
I also drill/mill a registration hole, usually at 0,0 to confirm any questions about lost steps.