Some Ideas for Ease of Use

[MontanaAardvark]

Now that I have my CNC G0704 running, I've been thinking of ways to make living with it easier and do things faster. I thought I'd put out a couple of ideas running in my head and ask you gurus what you think.

I'm not doing this for money, but a lot of time spent indicating the edges of a part for every part just seems like a waste of time. It's not hard, it's just tedious. Industry uses tooling plates or homing switches that always are (0,0) and I'm thinking of doing something like that. I've assigned a fixture (0,0) for several parts on a little project I'm building, making the front left hand corner of the fixed jaw on my vise into (0,0). All I have to do is put a piece in the vise, press it against the stop and it's ready to machine. Yeah, all my Y numbers are negative, but no big deal.

The issue is that the vise only holds a small range of sizes without changes. Something like this Sherline-sized tooling plate from eBay looks like the trick to do (no relation to the seller, don't know if it's any good, and all disclaimers). Set one corner as the reference point and go from there. Making or getting one for the G0704 might be a good exercise, although I think the clamping screw holes would have to be bigger due to the (much) higher power of the Grizzly over the Sherline.

Do any of you guys do anything like this?

The other thing I'm trying to improve is tool changing. I'd love a Tormach changer and the whole TTS, but they're like $4000 so that ain't happening (I am a retiree, after all). So I was thinking of getting a bunch of R8 end mill holders at $16 or $17, like this from LMS, and making a system of my own. Set the tools to all the same distance out of the holder (1" as example), and then when it's time to change tools, I'll still need to swap tools in the spindle, but they'll all be zeroed once the new end mill holder is in the spindle. I can replace the four sided nut on the G0704 with a regular hex head and stick a socket on a battery powered wrench to speed loosening/tightening. Or maybe a manual drawbar like Hoss shows on the DVD.

Again, anybody done anything like this?


Bob

 

[jbolt]

I have several tooling plates made from 1/2" aluminum plate or 1/2" mic 6 aluminum. I prefer to make my own since the pre-drilled hole locations may not line up well with a part. I also like to use dowel pins for locating stock. I machine the back edge and part of one side of the tooling plate for setup and reference. I keep a 3D CAD model of each plate and use them for creating the tool paths with the part on the plate. I also model the clamping fixtures so I can make sure I don't accidentally have a tool path go through a clamp. (learned the hard way)

I generally keep two 4" vises on my mill so I can extend the clamping range or run multiple parts. I also made a tooling plate from 3/4" aluminum that is machined to clamp in the two vises if I have a part that is outside the vise clamping range but don't want to take the vises off.

I use the TTS holders with a power draw bar. I like the TTS holders over the R8 end mill holders because they are faster to change plus they have drill chucks and ER collet holders etc..

In Mach3 I have a master tool, tool zero. Once that tool is zeroed in Mach3 all the other tools are given a number (corresponding to the tool in the CAM program) and their offsets are entered into the tool table in Mach.

 

[JimDawson]

Your plan sounds fine for fixturing multiple parts. For one-off parts, most times it's better just to locate the working edge or a feature on the part. I don't have a vice on the table for most operations, that's what the T-slots are for. If I need the vice(s), it only takes a couple of minutes to mount and tram the vice. To tram a vice, snug up one of the bolts, then just bump the vice with your hand as you traverse with the indicator using the jog buttons. Once you have minimal movement on the indicator (don't worry about getting it to ''0'', you are just looking for relative movement), then snug up both mounting bolts. Normally this only takes abouts 2 passes to get it trammed. I don't like keys for tramming the vice. Plan the operations to minimize tooling and fixture changes.

You can bolt a fixture plate to the table, then maybe use dowel pins to locate the part on the fixture plate. Use flat head screws to bolt the fixture plate to the table and countersink them extra deep to get them out of the way. If you need to mill the entire profile, then you can use shoulder screws to locate the part and then remove the shoulder screws after clamping. I normally try to design parts that have holes or some other area that facilitates clamping/bolting. MDF makes a great temporary fixture plate, you can also make a part shaped pocket to facilitate locating and holding. MDF is very resistant to petroleum based coolant, not so good with water based coolants.

End mill holders are fine, but trying to get the tools all the same height is difficult at best. Normally you would locate the tool height from a fixed point, maybe the top of the vice, fixture, part, or table, then plug the offsets into the tool library.

 

[cs900]

In Mach3 I have a master tool, tool zero. Once that tool is zeroed in Mach3 all the other tools are given a number (corresponding to the tool in the CAM program) and their offsets are entered into the tool table in Mach.

An alternative, and arguably better, way to set all your tool heights is to use a reference surface and a height gauge to measure the total tool height rather than having a master tool. This method would work with the TTS holders and could work with standard R8 holders as well.

In addition to using the corner of your vice as a work offset, I take that a bit farther. I have a step machined into some soft jaws for thin work holding. So one of my work offsets is to the corner of the step on the left (G54), another for the left corner of the inside of the jaw (G56) and I also have the same for the right side (G55 and G57). so depending on what side I need to machine I just change the work offset and go. Unless I'm trying to do something very accurately, it's very rarely that I indicate a part. Of course doing this you will need repeatable home switches which I think are a good idea any way.

 

[jbolt]

An alternative, and arguably better, way to set all your tool heights is to use a reference surface and a height gauge to measure the total tool height rather than having a master tool. This method would work with the TTS holders and could work with standard R8 holders as well.

The TTS tool holders register to the face of the spindle. All tools heights are measured (with a height guage) from the spindle mating surface to the tool tip and entered into a tool table. The master tool sets the zero to the spindle face. Each tool has a number (t#) and height offset (h#). Without a master tool (unless you zero the face of the spindle which is not always practical) there will be no offset tool height reference for any other tool unless you zero each tool individually as you use it.

An R8 holder registers to the taper so it would be difficult to measure the tool height out of the spindle.

 

[MontanaAardvark]

The TTS tool holders register to the face of the spindle. All tools heights are measured (with a height guage) from the spindle mating surface to the tool tip and entered into a tool table. The master tool sets the zero to the spindle face. Each tool has a number (t#) and height offset (h#). Without a master tool (unless you zero the face of the spindle which is not always practical) there will be no offset tool height reference for any other tool unless you zero each tool individually as you use it.

An R8 holder registers to the taper so it would be difficult to measure the tool height out of the spindle.

That's exactly the kind of thing I was thinking of. Setting the tool "stick out" of the EM holder is easy. Stand the edge of the holder on the edge of a 1-2-3 block, put the end of the cutter on the surface the block is setting on and tighten the setscrew. The question becomes is that surface in any way locked to the where the R8 taper sits in the spindle.

Thinking of it another way, there figures to be a reason that EM holders are 17 bucks and TTS holders are more like $80. I spent part of my career assuring repeatability in a totally different field (radio interference levels) and it left me with respect for how much money repeatability really costs.

<edit to add> The thing is, though, that setting Z heights is very easy compared to setting X and Y zero. As long as the center of the cutter is referenced to the center of the spindle, I'm not sure I care about setting Z heights.

 

[cs900]

The TTS tool holders register to the face of the spindle. All tools heights are measured (with a height guage) from the spindle mating surface to the tool tip and entered into a tool table. The master tool sets the zero to the spindle face. Each tool has a number (t#) and height offset (h#). Without a master tool (unless you zero the face of the spindle which is not always practical) there will be no offset tool height reference for any other tool unless you zero each tool individually as you use it.

An R8 holder registers to the taper so it would be difficult to measure the tool height out of the spindle.

maybe we are just confusing terminology. I think of a master tool as a tool that never changes (ie a pin gauge mounted in a holder). Using the method you just described (which is exactly what I was referring to and is the method I use every day) you do not need a master tool, you just need to make sure that height offset is called up in MAch3 before touching the corresponding tool off. You can use any tool to set the Z work offset, and as such you do not need a "master" tool, nor do you need to touch every tool off after that.

 

[jbolt]

Thinking of it another way, there figures to be a reason that EM holders are 17 bucks and TTS holders are more like $80. .

The standard TTS set screw holders are $22. ER collect holders are $35 https://www.tormach.com/store/index.php?app=ecom&ns=catshow&ref=TTS&portrelay=1

 

[jbolt]

maybe we are just confusing terminology. I think of a master tool as a tool that never changes (ie a pin gauge mounted in a holder). Using the method you just described (which is exactly what I was referring to and is the method I use every day) you do not need a master tool, you just need to make sure that height offset is called up in MAch3 before touching the corresponding tool off. You can use any tool to set the Z work offset, and as such you do not need a "master" tool, nor do you need to touch every tool off after that.

I think were talking along the same lines. Sure there many ways to accomplish the same thing. I prefer the master tool because that value never changes. I don't use a touch-off pad on my mill (I do on my router). I use a dial indicator in a TTS holder. When the indicator is zeroed to the part or fixture reference point the pre-measured value is already set in Mach 3 so I only have to pres the set z button. During startup Mach3 defaults to tool zero so that is the master tool.

Just my $ .02

 

[cs900]

I think we are as well. I do the very same thing on my lathe with a master tool as I'm too lazy to make a reference fixture to hold the tools so I can measure them.

My only concern is if you ever crash the indicator, you'll have to adjust all your tools to the new master. Not the end of the world, but annoying for sure, lol.