Accounting for Bit Diameter Variation

[erik_f]

Maybe I should know this after 6 years using the Shopbot, but until the last year or so I haven't been that interested or needed to be ultra precise. So the question is...is there an easy way to account for small variations in bit diameters without having to create a new .sbp file? I have thought about changing the proportions in the control software, but that would only work if the cutter was working on ONLY inside or ONLY outside cuts. I have noticed that spiral cutters tend to be on the smaller side of what they are supposed to be. A cutter undersized by .003" might not seem like much, but depending on the process that alone can add as much as .006" of thickness to a part. That coupled with run out, and machine flex, and backlash...it can screw things up pretty quickly. Anyone know of an easy way than going back into CAM and regenerating a new file based on the smaller bit size?

[magic]

What I do is run a test piece, measure, go back to the artwork and resize by scale or other- before I make any toolpaths.

and/or If you know your run-out and you put the bit to the caliper then you would have measurements before you design.

If you change the artwork, keep a copy of the original, off to the side.

[jerry_stanek]

You also can use the fill in sheet to change the offset to compensate for you bit

[knight_toolworks]

I don't think it is really possible. but maybe make toolpaths with the different bit sizes/ or use offset for the different bit size and save them as separate toolpaths.

[jerry_stanek]

the Sopbot software has the fill in sheet where you can input the offset

[erik_f]

Thanks for the replies. I don't think the fill in sheet in the control software will work if the file has inside and outside cuts. If the bit was too small and you changed the multiplier in the fill in sheet would it not make outside cut properly, but inside cuts too small? Let me know if I'm thinking about this all wrong. Making the multiplier smaller thanoe would have the opposite effect?

[carve_1]

Measure your bit with a michrometer, and enter that diameter for the tool you choose for the tool path. The software will make the accomidation.

[jerry_stanek]

I think he already has the tool paths made he just wants to compensate for bits that are not what was spec in the tool path.

[beacon14]

The short answer is no, not possible within Shopbot software except for very simple toolpaths like rectangles or circles centered at 0,0. For slightly more complex paths you could hand-write the code using variables for the offset, but it would be more trouble than just changing the bit diameter in PartWorks and re-calculating the toolpath.

Once you have completed and saved the project in PartWorks it really only takes a few seconds to edit the bit diameter and recalculate.

[erik_f]

Thanks that is what I figured. I suppose the more I think about it the more I see its a dumb question. There would be no way for the control software to know where or how to compensate based on the data in the cutting file.

[clueless]

It's not a dumb question at all. It's how most CNC machines work that use G-Codes. You create the tool path and you can change cutter sizes at will and change an offset value. For instance, if your tool path used a 1/2" cutter, you could put a 3/8" in and make an offset value change of 1/8" (or 1/16", depending how it was originally set up) and you are done. It works inside and outside, doesn't matter.

[erik_f]

I don't know anything about writing code but it would seem to be able to do this from the control software, the. Sbp files would get more complex. Maybe I'm picking knits at this point since it is pretty easy to go back and change it in aspire/partworks. My work computer and garage computer aren't the same. I try not to have anything but the control software on the garage computer. It just feels like there is a lot more room to mess things up by regenerating the file as opposed to just being able to enter in a simple offset.

[bcammack]

It's called "cutter compensation". The G-code is output with the positional info referent to the spindle centerline. The tool number references tool dimension info in the machine's internal tables when it gets a "compensate left" or "compensate right" and recomputes the proper spindle centerline.

Our Northwood Stone Center and OMAG Millx4 CNC routers do this, but they cost around $150,000.00 and $30,000.00 apiece, respectively.

[englert]

Many Cad/Cam applications have an option to post the G-code or CNC file with or without tool compensation applied. If tool compensation is not applied, then the control accounts for it and adjusts the tool path via G-code. In our case, the codes are G41 (comp left) and G42 (comp right). These codes apply the radius of the bit and adjust the toolpath on the fly. Since you've created a tool path and specified the offset in that toolpath the only way to account for a change might be to manually add compensating G-codes. That would or could be an extremely tedious process and prone to error.

So while the control may have the capability to adjust the toolpath for a change in bit diameter, the actual ability was restricted when the CNC file was posted from the Cad/Cam application. Your only alternative is to repost the file with the change in tool diameter.

If your control is capable of using tool comp codes and you want to, then post the file accordingly and setup your tool diameter.

Generally, we post our files with the tool offset already applied in the CNC file. The time to repost the file is typically insignificant.

Dennis Englert

[erik_f]

Thanks people