Bad T-slot guy learning to love his 1100

[flick]

Rather than resurrect the old T-slot thread, I'm starting a new one for my observations thus far.

It took me longer than expected to start using the machine because an expected slowdown at work didn't really happen (a good problem to have), and then the weather turned all nice and my dirt bike started looking pretty good on the weekends.

Now that I've had a chance to start playing with the machine, I'm really getting to like it. The few additional nuisances I've found so far have been minor, and easy to address. On a couple of occasions I have needed some technical support from Tormach, and though I have read consistently that they treat people well, I was still impressed with the level of service (not even a shipping charge for a missing part that I failed to report for over 3 months).

I've signed the waiver and gotten access to the full configuration of Mach 3. I really like the control software. Some areas are a little unpolished, but the level of configurability is 10/10. I wanted to improve the accuracy of the axis referencing routine to the extent possible with the stock hardware. My approach was a double touch on each switch, the second being at a reduced rate of travel.

This improves my homing repeatability from about 5 thou to within 2 or 3 tenths on each axis. I was forewarned by support at Tormach that I'm still using inexpensive switches, and it would be unwise to rely upon them if there is expensive or accurate work at stake, but I will still use it to eliminate unnecessary fixture touch offs for everyday stuff.

Other (control software stuff) that I've changed:
- Changed the X axis homing direction to positive
- Added a G90 to the M998 macro
- Put an M998 in the M6 macro
- Wrote a set of macros to cut involute teeth in the 4th axis with an endmill

As far as my original disappointment with the T-slots I've not yet found a situation in which they inhibit my productivity, and I've been too busy tweaking and tinkering to let them bother me much.

[zephyr9900]

Originally Posted by flick ...double touch on each switch, the second being at a reduced rate of travel. This improves my homing repeatability from about 5 thou to within 2 or 3 tenths on each axis.

That is impressive, flick. I'll need to look into that--not that I don't always indicate my parts, but I've always thought that a double-touch was really cool...

Originally Posted by flick ...I've been too busy tweaking and tinkering to let them bother me much.

That's a good attitude to have, flick. The PCNC is a really great tool, and very moldable to our individual needs. The shortcomings and rough edges are generally easily dealt with (I've stopped worrying about the base leaking coolant, and just keep a mop handy...) and I really enjoy using my Tormach.

Randy

[philbur]

Great to hear you are having fun. It would be interesting to get more details/photos of what you are doing on the gear cutting front, especially the set-up for cutting the involute using an endmill.

Phil

Originally Posted by flick - Wrote a set of macros to cut involute teeth in the 4th axis with an endmill

[ger21]

Originally Posted by flick My approach was a double touch on each switch, the second being at a reduced rate of travel.

Care to share the code for this, or at least tell us how you slow down the speed for the second touch?

[flick]

Originally Posted by ger21 Care to share the code for this, or at least tell us how you slow down the speed for the second touch?

Here's my "Ref All" button script:

DoButton(24)
DoButton(23)
DoButton(22)
While IsMoving()
Sleep(100)
Wend
SetParam("XRefPer", GetParam("XRefPer")/10)
SetParam("YRefPer", GetParam("YRefPer")/10)
SetParam("ZRefPer", GetParam("ZRefPer")/10)
DoButton(24)
DoButton(23)
DoButton(22)
While IsMoving()
Sleep(100)
Wend
SetParam("XRefPer", GetParam("XRefPer")*10)
SetParam("YRefPer", GetParam("YRefPer")*10)
SetParam("ZRefPer", GetParam("ZRefPer")*10)

The first 3 lines are the original script.

Originally Posted by philbur It would be interesting to get more details/photos of what you are doing on the gear cutting front, especially the set-up for cutting the involute using an endmill.

What I'm doing is calculating the tangent points of the involute curve, and cutting a sequence of nearby tangent points with the side of the endmill. It's really the same thing as generating the curve with a hob or gear shaper but more powerful because you can specify any parameter and cut it without changing tools or fixturing. As long as the endmill will fit in the root, it can cut the gear.

[zephyr9900]

Flick, neat homing technique. You know your way around Mach better than I do. Thanks for sharing it!

I have endmilled gears also, without a rotary table, with the same caveat as yours (endmill must fit between the teeth). There is an old DOS program called Geargen (Google geargn11.zip) that was intended for wire-EDM'ing gear mold cavities. If you use a negative "electrode overburn" (i.e. kerf) number, you can get it to generate gcode for endmilling the gear directly since the toolpath will be on the outside of the gear outline. It has options for 14.5 and 20 degree pressure angle. It can also output a DXF rather than the direct gcode.

Randy

[flick]

Glad you like the homing technique. I was a computer programmer for a couple years before the .com bubble. I'm rusty, but quickly getting the hang of VB.

Would you be willing to take some measurements and see how much it improves your homing accuracy? My estimates of accuracy/repeatability were based on simply jogging into the switches at various speeds and observing the DRO's. Perhaps there's a better way?

I like the idea of making gears using only 3 axes with geargen. Anytime you can do more with less, it's impressive.

I wanted to make a 4th axis macro to lift some of the practical limitations imposed by the 3 axis method, such as face width and root fillet radius. The 4th axis also allows helical cuts with ease.

I'm writing the macro to much more than standard gearing. I'm already doing arbitrary pressure angles. Eventually I hope to be able to specify arbitrary values for most any parameter imaginable.

Not that I'm that far yet. I don't have any post-secondary math education, so I'm stuck using high school trigonometry and Machinery's Handbook to figure out all the involute stuff, and I'm struggling with the trochoidal part of the tooth. This means that the macro is currently limited to rather large numbers of teeth.

[philbur]

Thanks for the reply. I see the process, but doesn't the necessary reach compared to the root width result in an unacceptably small diameter/length ratio.

Phil

Originally Posted by flick What I'm doing is calculating the tangent points of the involute curve, and cutting a sequence of nearby tangent points with the side of the endmill. It's really the same thing as generating the curve with a hob or gear shaper but more powerful because you can specify any parameter and cut it without changing tools or fixturing. As long as the endmill will fit in the root, it can cut the gear.

[flick]

Originally Posted by philbur Thanks for the reply. I see the process, but doesn't the necessary reach compared to the root width result in an unacceptably small diameter/length ratio. Phil

Don't mistake me for a gear guru, but I believe the root width/depth ratio becomes more troublesome with: greater pressure angles, larger tooth height ratios, and a higher tooth count. Profile shift is something I'm just starting to work on, but I believe it would have the same effect. I expect there are some profiles for which this technique would not be suitable but I've got a lot more work to do on improving the basics before I start looking for the practical limits of more extreme profiles.

[Scott_M]

Originally Posted by flick Would you be willing to take some measurements and see how much it improves your homing accuracy? My estimates of accuracy/repeatability were based on simply jogging into the switches at various speeds and observing the DRO's. Perhaps there's a better way?

Thanks for the code flick !!

I put a .0005 indicator on one of the limit switch blocks on the z axis and read the numbers by alternating between ref z and ref all ( I only put the code in ref all)

With the stock homing (ref z ) my repeatability was about .0005 to .0013 ( about 8 tenths)

With the "New Improved flick Double Touch Homing Technique" it cut it down to 2 or 3 tenths. But more times than not it was the exact same reading.
A very nice improvement !!
I think I will apply the code to the individual ref buttons as well.

Thanks again

Scott

[flick]

Originally Posted by Scott_M "New Improved flick Double Touch Homing Technique"

Have you trademarked that yet? J/K

I'm glad you find it helpful. I couldn't figure out how to apply it to individual buttons. I was hoping that I could do it that way, and then maybe the "Ref All" button wouldn't need any modification. How is it done?

[Scott_M]

Originally Posted by flick I couldn't figure out how to apply it to individual buttons. How is it done?

Let me poke around a bit and see if I can figure it out.

I'll report back

Scott