[Potatohead908]

So this weekend I am hoping to further my knowledge on CNC/machining stuff. I am pretty green so bare with me please! This week I completed Hoss's MAD system, received a couple of tts tool holders and made two of my own.

Here is what I have to work with:

• Inventor HSM
• 5 tools in tts holders
• G0704 cnc mill
• Mach3
• 2" indicator block
• tts collet
• Hoss's design MAD

What I hope to do this weekend is learn how to build a tool table in Mach3 and hopefully be able to export it to Inventor HSM. I'm not sure where to start with what I have at hand. Using the 2" indicator block can I indicate the height of the mill head then indicate the tools in their tool holder to get the tool height? It seems this would be accurate. I would be using the measurements on the Mach3 DRO to get the differences and that would be the tool's height. Will this work accurately? If not do you have another suggestion other than buying some sort of height indicator like Tormach sells.

Thanks for any input.

[AVRnj]

What I do is measure each tool in its holder using the tormach granite block and a digital height gauge. I store the tools in the Mach3 tool table. I try to logically arrange my tool table so that I have room for growth, and they make sense to me. So for example, my spot drill is tool 1, and my drill bit tooling is from 5-25, leaving spaces in between because I don't have that many. My end mills range from 35-65, my super fly face mill is 75.

I have the same table replicated in HSM, but I did not import it, just created it manually, but I only have around 30 or so tools, so it was not a big deal, but it is probably easy enough to do.

I then make sure for my Z height when I set it, I have the right tool selected in Mach3, and the rest is handled by HSM. It is pretty easy, but I would recommend cutting in wood or wax the first couple of times to make sure you have everything set properly and your Gcode is being processed the way you want it to from HSM

[Potatohead908]

Thanks AVRnj. I don't have a granite block or digital height gauge so I need a work around on that. The logic you have used for the table itself makes sense and I will use what you have done. I haven't gotten that far and I only have a 5 tools right now.

[AVRnj]

Thanks AVRnj. I don't have a granite block or digital height gauge so I need a work around on that. The logic you have used for the table itself makes sense and I will use what you have done. I haven't gotten that far and I only have a 5 tools right now.

I think the granite block and gauge are the best ways to do it, but you can probably get creative with a piece of stock, and putting each tool in the spindle while touching the stock and noting the differences in z.

I don't think the actual height matters, only that the offset between the 2 is exact.

[Potatohead908]

Ok that is what I was planning. I have a 2" block from shars that has an indicator built in. Drop the tool on top and travel down to 0" will put me at 2" off of surface/bed.



shars.com - Precision Magnetic Z Axis Setter 2quot Height x 0001quot

[AVRnj]

Ok that is what I was planning. I have a 2" block from shars that has an indicator built in. Drop the tool on top and travel down to 0" will put me at 2" off of surface/bed.



shars.com - Precision Magnetic Z Axis Setter 2quot Height x 0001quot

That should work well, should work at least as well as the granite block and the height gauge. I use a digital height gauge, and can turn it off and then back on, zero everything out again, and be a few tenths of a thousandth off, I would think you should be able to get great accuracy with that.

[Potatohead908]

Sweet! I will report back with what I find. I am hoping to create g code from HSM and make a part this weekend. If I can get it to work I will be stoked!! I may have some more questions for you since you have the same software I have....if you are good with that?

[AVRnj]

Sweet! I will report back with what I find. I am hoping to create g code from HSM and make a part this weekend. If I can get it to work I will be stoked!! I may have some more questions for you since you have the same software I have....if you are good with that?

Happy to help anyway I can. I will emphasize though that I would personally not cut in metal until you are really sure you are measuring things properly, and your post processing properly. When I first started using TTS I had a bit of trouble getting the post processing right so the offset would be correctly applied. I am not an expert by any means, so others may be able to help as well.

[rs4race]

Ok that is what I was planning. I have a 2" block from shars that has an indicator built in. Drop the tool on top and travel down to 0" will put me at 2" off of surface/bed.



shars.com - Precision Magnetic Z Axis Setter 2quot Height x 0001quot

I need to get one of these. It looks like it would make offsets easier.

I use a tts edge finder for tool 0 and use that to set zero. For my tool offsets in mach I use a 123 block and lower my tool until I cant slide the 123 block under anymore. This is usually 1.999 in. A little math for the offset and store it in mach under that tool number. That sets up the tool offsets in mach.

In Inventor HSM the only tool information you really need is the cutter geometry (type, flute length, diameter, and approximate stickout) and the tool number. Then you can program your tool paths, post process using mach 3 post. All thats left is to load your program in mach and run it.

[pippin88]

Remember that you have tool offsets and work offsets.

You'll need to tell the controller (Mach3) where the workpiece is. This is done by zeroing G54 in X,Y,Z as appropriate. But these are affected by tool offsets. And tool offsets are relative to something. So usually you pick a reference tool that will have no offset (most commonly a probe if you use one) and then set offsets relative to that.

You can just have the controller aware of tool length. Your CAM doesn't need to be aware, it just says load tool 1 with offset from table and go to Z10.

I use linuxcnc. It allows for tool numbers up to 99999. So I use a human readable code for my numbers. The first digit is what type of tool - 1 for endmills, 2 for ball nose, 3 for drills. The next numbers (next 2 digits for EM, next 3 for drills) encode size. The fourth digit for milling cutters is number of flutes. The final digit is for length / special.
So 10840 is an 8mm 4 flute standard length end mill, 31270 is a 12.7mm (1/2") standard drill.

[SCzEngrgGroup]

"And tool offsets are relative to something. So usually you pick a reference tool that will have no offset (most commonly a probe if you use one) and then set offsets relative to that."

That approach has always impressed me as rather convoluted, as it requires adding/subtracting tool lengths to get the value you enter into the tool table. And, if your reference tool length changes, the entire tool table is wrong. Instead pick ANY tool of known length. For any TTS tool, this length is the distance from the "ring" that seats against the spindle nose to the tool tip. Move the tool down until it just touches the Z "zero" of the workpiece (usually the top of the workpiece). Set the Z DRO to the length of THAT tool. Your Z fixture zero is now set to the spindle nose. For ALL tools, the value you enter into the tool table is simply the length of that tool, from the "ring" that seats against the spindle nose to the tool tip. It is then also trivial to verify your tool lengths before hitting CycleStart after a tool change. After the G43 is executed, the Z DRO will show the exact distance from the tool tip to the top of the workpiece. For the first run of a given job, I use a tape measure to make sure this distance is correct after each toolchange, before hitting CycleStart. So, if I made a mistake entering a number in the tool table, I'll know BEFORE I crash the tool, or waste time cutting air.

The TTS surface plate, or any similar plate with a 3/4" hole in it, combined with a height gauge, makes setting tool lengths absolutely trivial. I measure all tools using the TTS surface plate and height gauge before each job - it takes under 2 minutes to do a dozen tools - in other words, its lost in the noise compared to the job run-time.

Regards,
Ray L.

[pippin88]

Ray, that's an added benefit of TTS I hadn't appreciated.

I've got TTS recently, but not actually been using tool table and Z offsets yet (just touching off per tool)

So the tool ring is zero and all tools are + relative to this.

[Potatohead908]

I don't have a height gauge. I'm pretty sure that all I will need to do is drop the nose of the mill onto my 2" block, zero that, then build the tool table for the limited tools I have in tts form on the same 2" block. Then when referencing my Z zero for a part I can pick a tool, place the 2" block on my part, drop the tool down until the block reads zero and reference in Mach3 using 2"'s as my gauge block height.

Ray I think you just saved me some head scratching on referencing Z zero on a part. For some reason I was thinking Mach will know what tool I have loaded but that is not the case when referencing. Please correct me if I am wrong.

[pippin88]

Potatoe, that's what I was trying to get at with work offsets being affected by tool offsets. Once you have all your offsets in your tool table, you load a tool with it's offset (eg T1 M6 G43). You then zero the top of the workpiece (if that is your zero, it's most common, but zero might be your fixture or similar).

[Potatohead908]

Ok pippin88, I will hopefully get a chance today do this and hopefully it will sink into my brain then. I see what you are saying. I'm still a little confused as to why Ray said to compensate for the tool height by entering the height of the tool to get your zero. Maybe I'm understanding his post wrong.

[SCzEngrgGroup]

Ok pippin88, I will hopefully get a chance today do this and hopefully it will sink into my brain then. I see what you are saying. I'm still a little confused as to why Ray said to compensate for the tool height by entering the height of the tool to get your zero. Maybe I'm understanding his post wrong.

You can use any reference point you like, but the spindle nose is the most logical choice. And, with TTS tooling, by far the most convenient and easily-measured. If you zero to any other reference, then all your tool lengths become differences from whatever reference you've chosen, rather than absolute, direct-measured values. With no tool installed (i.e. - a zero-length tool), the spindle nose should be just touching the top of the workpiece when Z=0.000. For any other tool, with the correct tool length applied, the Z=0.000 position will put the tip of the tool on the top of the workpiece, and the spindle nose above the workpiece by the exact length of that tool.

Regards,
Ray L.

[Potatohead908]

Ok that makes sense. It will work either way however it maybe more logical to use the mill nose to zero off of as it is your true zero when using tts type tooling. I'm sure there is more too it but I don't know what I don't know. Thank you.

[SCzEngrgGroup]

Ok that makes sense. It will work either way however it maybe more logical to use the mill nose to zero off of as it is your true zero when using tts type tooling. I'm sure there is more too it but I don't know what I don't know. Thank you.

I do all my fixture offsets by probing, using a "probe" that is a 1/4" brass rod with a TTS gauge length of exactly 3". The touch-off macro touches off on the top of the part, then sets the Z DRO to 3", and I'm done. X and Y are done the same way, except after touching off the macro sets the X/Y offsets to +/-1/8", depending on the direction of probing. Setting up X/Y/Z fixture offsets takes all of about 30 seconds. Another 60-90 seconds to measure all the tools, and enter the offsets into the tool table, and I'm ready to run.

Regards,
Ray L.

[pippin88]

Potato, it's probably easiest to just have a play around with the mill and offsets while jogging etc to get a handle on it.

You just need to be aware if there is a tool offset in effect or not when you zero G54 (the standard coordinate system).
It had the same result whether you zero with the empty spindle nose or a tool with measured offset loaded.
For instance if you have a tool with 1" stickout from the TTS shoulder and a tool with 2" stickout, you can zero with either of them if you load the tool length offset (G43) for the correct tool. Problems arise if you have the wrong tool length offset (measured incorrectly, or you have the wrong tool loaded) which results in air cutting or an excessively deep cut, or worse a crash.

Ray, is your probe a simple close the circuit (ala touch plate)?

[SCzEngrgGroup]

Ray, is your probe a simple close the circuit (ala touch plate)?

Yes, The "probe" is just a piece of 1/4" round brass in a TTS set-screw holder, and it contacts a piece of PCB material (connected to a BOB input with a stiff pull-up resistor) placed appropriately between it and the workpiece. It's cheap (practically free), and if I crash it, costs nothing to replace.

Regards,
Ray L.