[ToolChatter]

Hi Folks,

Cut my first CNC chips this weekend and feeling pretty stoked. I'm working with BobCad for Solidworks and using a Centroid controller. I haven't been able to figure out the best way to zero Z after a tool change. I have QC40 tool holders, so I suppose I could measure all the tools beforehand and program in fairly accurate tool lengths, but would really prefer to set a new Z zero by jogging after the tool change. What do people with R8 spindles do since they don't really know exactly where a tool is going to wind up? This may be a stupid question, but I was once told that there are no stupid questions, only stupid people, and I'm pretty sure I already qualify as that.

Thanks!
Tom

[Kenny Duval]

I went the route of a fixed touch plate and use my touch probe as my master tool. G54 is set against the touch probe and all tools are measured during the tool change via the touch plate. The offset is the difference between the measured length of the touch probe and the measured length of the tool.

You can see it in action in this video I did to track down an issue I was having.


You can turn the sound down to not bore yourself to sleep.

[ToolChatter]

Cool. So you have the ability to change the tool length in the program on the fly? I don't think my controller is setup to do that. Or have I just not found that functionality yet?

[Kenny Duval]

Yes. Mach Standard Mill can do it out of the box and that's the interface I'm running. It sits on top of Mach 3. I believe you have to install and configure a few bits if you are using the stock Mach 3 screens. The information is either here or on the Mach 3 forums that you seek.

[ToolChatter]

I have an old M-40 controller that doesn't appear to allow this.

My plan is to load each tool and touch off on the part and record the offset for each one from the longest tool. Then I'll enter the tool data into BobCam with the length of the longest tool being approximate but the difference between all the tools being accurate.Then I'll set up the WCS to be at the top of the part. The problem I'm having with that is that I can't figure out how BobCam uses this info. I ran a program with 2 tools where the longer tool is used in the first operation. I set the WCS at the top of the part and the first operation worked fine. The 2nd tool was about .25" shorter, which I had entered into the tool info in BobCam, and it went to the same place as the first tool, so the feature was .25" too shallow. I tried using the "override offsets" option in BobCam, but when I entered the diameter offset of 9.52mm (for a 3/8 endmill), it changed it to 10. Anyone know why it's doing that? Anyone know why it went to same Z position for 2 different length tools?

Thanks,
Tom

[mmoe]

I have an old M-40 controller that doesn't appear to allow this.

My plan is to load each tool and touch off on the part and record the offset for each one from the longest tool. Then I'll enter the tool data into BobCam with the length of the longest tool being approximate but the difference between all the tools being accurate.Then I'll set up the WCS to be at the top of the part. The problem I'm having with that is that I can't figure out how BobCam uses this info. I ran a program with 2 tools where the longer tool is used in the first operation. I set the WCS at the top of the part and the first operation worked fine. The 2nd tool was about .25" shorter, which I had entered into the tool info in BobCam, and it went to the same place as the first tool, so the feature was .25" too shallow. I tried using the "override offsets" option in BobCam, but when I entered the diameter offset of 9.52mm (for a 3/8 endmill), it changed it to 10. Anyone know why it's doing that? Anyone know why it went to same Z position for 2 different length tools?

Thanks,
Tom

I don't think that will work. Bobcad uses the tool length info mostly to allow the simulation to properly evaluate the toolpath for collisions between stock and the tool holder, etc. The proper place to enter the difference between tools is the tool table in your controller. I doubt there is a controller out there that does not allow you to use the tool table. You start with a specific tool that you feel is the "zero" tool (usually the shortest), then enter the difference in length between the zero tool and the other tools under each tool number. Bobcad will then use whatever format your controller requires to specify to the controller which tool table entry to use, usually an "H" value for tool length compensation. H1 will use the compensation you enter for tool 1, H2 for tool 2, etc. Every controller is a little different in how you specifically need to format the code, so you'll need to get that info in order to configure your post processor to automate it. Bobcad pretty much programs all the tools the same, as if the end of all the tools is at zero, but then uses the tool length compensation you enter at the machine to even it out. Hope that makes sense.

If you want, you can also just program each tool as a separate program, then enter the difference in tool length as a new Z value in the work coordinates. After you finish one program, let's say that the next tool is 10 mm longer than the tool that just finished. You can just change your Z value to be 10mm lower than it is. If your Z moves positive as it moves up and negative as it moves down, and the Z value in G54 work coordinates were for example "+75.2mm", you could just change that work coordinate value to "65.2mm" and the tool tip for the new tool should match the old one. If the tool is shorter by 10mm, you would add 10mm to the Z value in that case. If the Z move negative in the up direction and positive in the down direction (if you are at Z0 and move to Z4, it moves down by 4 units, while Z-4 moves up 4 units), you would do the opposite.

[ToolChatter]

Ahhh...interesting. Clearly I had the wrong idea of how this works. So the "override offsets" fields are looking for a tool number, not an actual offset, which is probably why it rounded it to the nearest integer. Ok, I'll try to figure out how to enter the tool info into the controller. Thanks!

[mmoe]

You'll also need to know the format the code needs to be in for tool length compensation. This can be a little different from controller to controller, but Bobcad can accommodate the differences in the post processor. If you post the format you need, we can help you adjust the post processor to match.

[JEST]

Even though your controller is old by todays standards, you should be measuring your tool length before running...
The controller has a tool database and you must populate it with corresponding data. The measurements can be the same for both Bob and your Centroid controller...

The controller expects you to define "zero" as it relates to home AND as it relates to your part (or fixture).
The tool diameter is pretty straight forward. Length can be confusing to some, but is actually just as obvious, once you understand the process.

See this PDF file for reference http://www.elrodmachine.com/PDF/M-Series%20Operator's%20Manual%20v3.04.pdf

Chapters 4 and 5 should help considerably!
Good luck.

[mmoe]

You should also be able to use tool length compensation without using tool diameter machine compensation. Some prefer entering the tool diameter in the tool table and letting the machine compensate, while other may prefer letting Bobcad make the tool diameter compensation in the software. My preference is to let Bobcad do it so that I can see that it's correct, but there really is no right or wrong. It's easier to compensate for tool wear using machine compensation, which is nice for resharpened tools or applications where you are measuring your tools even when new. I run a commercial CNC router, so if the tool is new and supposed to be .5", that's as close as I'm going to bother getting since the tool is probably more precisely made than the machine's accuracy (even though it's a very high end router). For some vertical machining centers, it would make a lot of sense to measure every tool and let the machine compensate since they can hold a tight enough tolerance to make it worthwhile for more precisely machined parts.