Ordering Pro 4824

[LeeWay]

Swapping the red and black wires fixed it up.
I got the phenolic table installed today. I am wanting to install the blast gate right at the spindle, but I will have to sleep on it. That would be the easiest place to get to when we run the sanders. It will need a bracket. I'll see what I can come up with.
Here is a picture.
I will surface it tomorrow. I had to remove the end stops. Too close for comfort.

[LeeWay]

It seems with the router setup in this configuration, I only get 22.25" of usable table in the X axis. Now this really isn't a problem for me. It might be a surprise for some. My production blanks are 16" by 48". To get the full work area, I would have to slide the table this way and either add another extrusion to the front and two small ones on the back or use a few of the brackets like I used under the bed. I can surface the entire 2' x 4' spoil board with this bit though.
Since I don't actually need the extra travels, I think I will optimize it at 22.25". Cut the spoil boards to that size and go with it. I still have the larger plasma cutter than I can route out larger stuff with if needed. Like the Tormach lathe, I will optimize it for our production.
The new spindle is probably one reason some of the table space is lost. It has a double plate mounting system, however it has an eccentric tram aid designed in. Sweet spindle too, so I am cool with that trade off for space.

I will lubricate the racks and square up the gantry.. Then set out to surface it.
Gwizard tells me my spindle will not go slow enough. This is a 1.5" 2 flute surfacing bit or face mill. I plan on a .01" DOC @ 50% step over and go about 60 IPM. 10 degree ramp. 8000 RPM. I couldn't find a Manufacturer suggested surface speed or chip load. GW says this is a .003" chip load.
I'll search around to see if I can find a similar tool with factory recommendations.

[LeeWay]

Oh and I forgot to mention that I will check the Z height around the sheet first and set Z zero at the high point in the surface. Otherwise if it is off much, calculating DOC and feeds and speeds might not be optimal. I have some small thinner pieces of this material here. I used to make push sticks out of them. I may try out a piece of that with this recipe first. I think the biggest issue will be burning. If I can keep it from doing that, I'll post that recipe.

[LeeWay]

Tools Today has some F&S charts for most of the tooling they have. Simple formulas for the most part and give a range. You can make it jive with GWiz. You can make it do a wide variation if you want. You can do that with Gwiz as well with the turtle and hare slider.
Test cuts will tell me just as much on some scrap pieces.

[LeeWay]

Looking over the thread, it took about 2.5 weeks to get this together doing most of it by myself in the evenings for an hour or two. I did a lot of peripheral stuff for it as well. That included running the power lines for it and an extra for the DC and vacuum pump. Running the duct work. Making extra safety brackets, grommets, etc. Making the base more solid and adding legs. Redoing stuff a couple times. Trouble shooting some minor issues. Thats not too bad. It may have only taken a day or less with a couple of us working on it if we had been prepared for it.

[LeeWay]

I was able to get the phenolic surfaced okay. I cut most of it at .015" DOC 12000 RPM and 150 IPM. Seemed to do pretty well right there. I started out slower and increased past that spot too, but the best was right there. Now there was quite a bit of resonance with this. Where the sheet has not support underneath, it was notably a different cut. Where the bracing under the phenolic is was very smooth cuts. Where it was not supported is not quite as nice. I had to make several passes as well. I wound up taking about .06" off the deepest part and just shaved the low part. She is flat now.

I did square up the gantry and lube the racks and rails. One and a half turns on the X home side sensor was all that was needed to square the gantry.
I also took the time after the first pass to tram the spindle. I had to adjust it ever so slightly using the tramming aid that is built in. The bit cuts perfectly flat now.

I did design the bracket for the blast gate. It actually mounted to the Z extrusion, but snugs up around the spindle too. Works great. The prototype dust shoe worked very well It captured 99% of everything. Probably even 99.5%. At some spots, it was hanging off the table, but still catching the dust. That was cool to watch.
I used the 3" brush on it. The key to not letting the brush get into the bit is to adjust the height of it according to the bit length. The brush was about .125" longer than the bit in this case. No chance for it to get into the bit. Even though it was a 1.5" tool.
I don't have a collar made yet. I didn't design one into this prototype, but with that and a couple brush lengths on hand, you should be covered for most applications.
Oh and that light ring works great. I only have it attached temporarily in this prototype shoe, but that will be a desirable option for most I think.


I will see how well it works with a small tool cutting the vacuum grid and insert holes today. Then back to the surfacing bit for the "spoilled" board. Good name for an MDF sheet.

I am pretty pleased with everything about it so far. Very smooth movement. Very solid on the base I put it on. Spindle is very powerful and quiet. Barely got over room temerature, so staying cool. I expect it will do a great job for us. I did snap a few pictures, but left the camera in the shop.
I will get some more progress pictures posted later.

[LeeWay]

It is coming along.
Initial stuff going as planned. The dust collection was inadequate for the vacuum grid job.
It would not pull all the swarf out of the grooves. It was getting maybe 60 to 70 %.
On the polycarbonate however, it was far worse. Heavier chips. It was only getting about 10% pickup. That will not do.

This was with a 3" brush though. I could have used the 2" brush and had a little better performance I think.
Once I get the second prototype done with the extension collar, I will do some dedicated skirt testing.
I figured out that for the time being, I can run my Home made collector on this.
I just have to move it from my old shop to the new. It won't actually be outside, but in the garage with the plasma cutter. Out of the rain just like it is now.
I will spring for a bigger cyclone sometime after the first of the year and put it in the same location.
The home made one pulls about 1575 CFM.
I forgot how many inches I used when I tested it. About 3 times the CFM of this little collector.

Not sure how well my vacuum pump is going to work yet, but this little blower may get added onto that system for extra volume.

The phenolic table doesn't look flat in the photo's but yoy could only barely feel any ridges and those where where it is unsupported. It really resonated when surfacing those spots.
More supports would have been desirable.

[gfacer]

I'll be very interested in how the dust collection goes...as I have largely given up on that due to heavy chips and less vision (and we are a lot like a job shop so things are different every job so seeing what is happening reduces scrap).

Love to see a success with that!

[LeeWay]

Kind of embarrassed to say it, but the DC bag was half full already. Once we emptied that out, it is picking up the polycarbonate swarf well too.
Still with the 3" brush. That is a positive sign I think.

[LeeWay]

I had an odd thing happen last night with this. I did an autozero move with the touch plate. It did what it should have. Touched, and retracted and set the Z zero height. I removed the plate and Z started moving back down. Unfortunately I caught it just in time to see the bit break. Plowed it right into the material.
I have used the touch plate a few dozen times so far and had not seen it do that before. My Estop is right there on this machine where we touch off from, so I can catch it in the future now that I am aware it can happen, but what might have caused that? If the cause cannot be determined, maybe I can put an auto estop in after the tool sets it's height? There were no buttons pushed anywhere that could have caused it, but we are using a little wireless keyboard simply for jogging the axes. That is puzzling for sure and will be watched closer.

Other than that, the machine is doing good. I have not calibrated the X and Y axes yet, however our new parts are coming out with the profile and the holes lined up perfectly with the parts we were having made elsewhere. If fact if you paired them up together, you could not tell a difference. Theirs was always having issues with the depth of the dados. Ours are identical across all parts.

So far I am pretty pleased with the machine. It is flat enough that we can do onion skins on the parts rather than tabs. That makes machining and clean up a bit faster. The deburing tool takes care of the onion skin. The machine itself camphers the inside edges, so we only have to do the bottom side. That is something we did manually on both sides before.

This same technique leaving a thin skin around the profile will help us out when we do get the vacuum table setup. Right now we manually drill the holes in the blanks several at a time and then screw each one down. Vacuum table would eliminate those steps.

[CRP]

I removed the plate and Z started moving back down.

Hi LeeWay,

Could you paste the script you are currently using for Auto Tool Zero? Our touch plate instructions (start with step 4) show how to open the button script macro from Mach3 Auto Z Touch Plate Instructions | CNCRouterParts (as well as the script we provide).

The only things that come to mind offhand are;
1) Sticky Keyboard key (not unusual in CNC/dusty environments)
2) Auto Zero script accidentally pasted in to the button script macro window twice (though it would probe twice every time in that case)

-Nathan

[LeeWay]

Here is the button code. I took this directly from the USB stick that I copied and pasted it with on the laptop running the machine.

Message( "Auto Zeroing..." )
If IsSuchSignal (22) Then
Call SetDRO( 2, 0.00 )
code "G31 Z-3 F20"
While IsMoving()
Wend
Call SetDRO( 2, 1.00 )
code "G1 Z1.5"
End If

It has done it twice so far. I did have a laser mouse sitting on top of a few keys on the laptop. That may have had an impact. I took that mouse out of the system.

Yesterday was a new problem. I could not get the AZ button to function. Restarted and homed a few times. Completely powered everything down and retried. It would still not work.
Then I used a backup XML from a couple days prior. Everything worked as it should then. This is confusing for me. My Plasma cutter is doing the same thing sometimes. It has done it three times so far. The XML gets corrupt somehow and the torch will not fire. Restore an older version and all is well. Totally different types of computers. Both running the same version of Mach 3 though. 3.043.062. That should be the most stable version. I run it on my mill too, but without that issue.

It only takes a minute to swap out the XML, but you loose time figuring out that it is required at that time.

On a side note, the first day, my Son was trying to run the machine. He would have trouble when auto zeroing a new tool. I asked him what he was doing wrong. He said I do it the same way as you do.
I said show me. He placed the puck on the mdf top and proceeded to auto zero there. I let him know the error. Honestly though, I think he only watched me when I was surfacing the table and spoil board. I don't think he actually watched me autozero the material to be cut. It's all good now. I really do like that tool BTW. Very easy and accurate. I will be getting one for the mill as well.

Oh and one little note. I had the feed rate overridden to 300% at one point testing the different cut results at different speeds. Well auto zero goes three times as fast too and is fast enough to depress the spring some before stopping.

Always look to see if the feed rate is at 100% or less. Never more.

[ger21]

I would look for a more robust auto zero script.
That one is susceptible to doing different things depending on the motion mode that Mach3 is currently in.

It's also not the most accurate, as it doesn't allow for deceleration when the tool hits the plate.

[ger21]

Oh and one little note. I had the feed rate overridden to 300% at one point testing

You should never run Mach3 at feedrates over 100%. This is a known issue that can affect the smoothness of your motors at higher FRO amounts. It's probably OK to go to maybe 150%, but anything higher may cause issues. If you are in the habit of always turning up the FRO, then you should program the feedrates higher and run with the FRO turned down less than 100%.

[LeeWay]

Thanks Gerry. Do you have a suggestion for the button code?

As for the feedrate thing, I was only testing out some different types of router bits at different RPM's and feeds at different DOCs. Something I have not been able to do before with a PC690 router. I was looking for light fluffy chips. Nothing fluffy at all about PC chips. I did get some nice curl;s at one point, but it was rough cutting. We never change the rates when I am running production, so all that code is correct and optimized already.

I have always used solid carbide two flute straight cutters from Onsrud. II picked up a couple single flute straight carbide cutters to try. I also picked up a two flute down cut.
I have ordered a couple O flute down cut from Onsrud to try out as well. We are getting cut marks on the edge of the plastic. Doesn't matter in the dado's, but does effect the profile. We have to sand them with 240 grit belts to smooth them out.

The down cut didn't work well enough because we were leaving an onion skin. We will be using tabs though. They require much less clean up and are much easier to snip out of the skeleton.
When the o flutes get here, I will do a little more testing of both using tabs.

[ger21]

To get a really good finish, you'll probably need to do a light finish pass at a slow feedrate.

The code I use requires my screenset to work, but there's a sticky thread in the router project log section here that has a lot of info on auto zero scripts.

[dgage]

To get a really good finish, you'll probably need to do a light finish pass at a slow feedrate.

The code I use requires my screenset to work, but there's a sticky thread in the router project log section here that has a lot of info on auto zero scripts.

Gerry,

Since I've never used Mach 3 before, starting with the your Mach3 2010 screenset would be a good option. Is there anything I'd be missing by going with your screenset vs the default Mach3 screen? Thanks.

David

[ger21]

There are a lot of things in Mach3 that are not in my screenset. Whether or not you'd miss them would depend on if you need them.

Personally, I highly recommend learning how to use Mach3 with the default screen before using the 2010 Screenset. That way you can refer to the manual and the thousands of youtube videos if you have any questions while learning.

[dgage]

There are a lot of things in Mach3 that are not in my screenset. Whether or not you'd miss them would depend on if you need them.

Personally, I highly recommend learning how to use Mach3 with the default screen before using the 2010 Screenset. That way you can refer to the manual and the thousands of youtube videos if you have any questions while learning.

Good advice Gerry. Thanks.

[LeeWay]

Is there a particular line or two that I could add from say the Aussie Tool setter thread that would add needed enhancements to the stock CRP button code?

Here is the stock code again.



Message( "Auto Zeroing..." )
If IsSuchSignal (22) Then
Call SetDRO( 2, 0.00 )
code "G31 Z-3 F20"
While IsMoving()
Wend
Call SetDRO( 2, 1.00 )
code "G1 Z1.5"
End If


This is the code from that thread.
I know this is in metric. I am just using the standard Mach 3 screen for now.

DownStroke = -25 'Set the down stroke to find probe
DownFeedRate = 100 'Set the down FeedRate
RetractStroke = 10 'Set the retract Stroke
RetractFeedRate = 300 'Set the retract FeedRate

CurrentFeed = GetOemDRO(818) 'Get the current feedrate to return to later
CurrentAbsInc = GetOemLED(48) 'Get the current G90/G91 state
CurrentGmode = GetOemDRO(819) 'Get the current G0/G1 state
PlateThickness = GetUserDRO(1151) 'Z-plate thickness DRO

If GetOemLed (825)=0 Then 'Check to see if the probe is already grounded or faulty
DoOEMButton (1010) 'zero the Z axis so the probe move will start from here
Code "G4 P2" ' this delay gives me time to get from computer to hold probe in place
Code "G90 G31 Z" &DownStroke &" F" &DownFeedRate 'probing move
While IsMoving() 'wait while it happens
Wend
ZProbePos = GetVar(2002) 'get the axact point the probe was hit
If Abs(ZprobePos) <= Abs(DownStroke)-0.1 Then 'Check if the probe has been found
Code "G0 Z" &ZProbePos 'go back to that point, always a very small amount of overrun
While IsMoving ()
Wend
Call SetDro (2, PlateThickness) 'set the Z axis DRO to whatever is set as plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
Code "G1 Z" &PlateThickness + RetractStroke &" F" &RetractFeedRate 'retract
While IsMoving ()
Wend
Code "(Z axis is now zeroed)" 'puts this message in the status bar
Else
Code "G0 Z0" 'retract to start pos
While IsMoving ()
Wend
Code "(Z-Plate not found, check connection or stroke and try again)" 'puts this message in the status bar
End If
Else
Code "(Z-Plate is grounded, check connection and try again)" 'this goes in the status bar if aplicable
End If
Code "F" &CurrentFeed 'Returns to prior feed rate
If CurrentAbsInc = 0 Then 'if G91 was in effect before then return to it
Code "G91"
End If
If CurrentGMode = 0 Then 'if G0 was in effect before then return to it
Code "G0"
End If
Exit Sub