# First pass is too deep



## OCEdesigns (Jan 31, 2019)

I have not noticed this before but in this project it was my first attempt at milling Aluminum. The plate is 1/8" thick (0.125) and 18"x18" I set everything up to use Virtual Zero. I'm running V-Carve Pro 9.5

I set it to a maximum cut depth of 0.030 and the end mill set to maximum pass depth of 0.010 for a total of 3 passes. See pics

The problem is the first pass was 0.035! The next 2 passes were correct at 0.010 each. I ended up with 0.055 total depth. The total depth I was OK with because I had enough material thickness to work with but the initial pass of 0.035 caused the end mill to "Dig" in or be pulled down into the material which caused a few imperfections in the sign. I checked a few tutorials and they all have the Start Depth at 0.0. And I did set it up to use the material surface for starting point.

Any ideas why my first pass is going way beyond the set point? What am I missing?


----------



## OCEdesigns (Jan 31, 2019)

The picture of the R is a test piece I tried after I made the sign and it did it again. (The R is actually from the sign. I just set it up separately on another piece of material)


----------



## Pro4824 (Oct 17, 2015)

Sorry I'm no help but at least you're not alone. My first aluminum cut did the exact same thing. I never did figure it out. Broke 2 bits, rebooted, recalculated everything and then it worked fine.


----------



## UglySign (Nov 17, 2015)

Make sure you're using a coolant cutting Alum.
Some do get by on plain air others do WD40.

I hate the WD40 smell and the mess it leaves.

Actually surprised at the cost of the FogBuster

Pretty soon I'll be cutting alum but not looking forward to
giant mess that'll be left all around the machine.

When doing the Alum cut setup, wouldnt be just the same as you
normally would? just a less than thru cut?

Can that program do side-to-side cuts? They look better
than the spiral if paint filling.


----------



## OCEdesigns (Jan 31, 2019)

UglySign said:


> Make sure you're using a coolant cutting Alum.
> Some do get by on plain air others do WD40.
> 
> I hate the WD40 smell and the mess it leaves.
> ...


I did the WD40 and it worked real well. I actually prepped the entire area pretty well to keep the mess as contained as possible. I can do the side to side cuts and have done that several times in wood. My only issue with this was the initial cut of 0.035 depth instead of the programmed 0.010 depth.


----------



## honesttjohn (Feb 17, 2015)

Check your Safe Z and Home position settings. 

Does the preview show the deep cut?


----------



## OCEdesigns (Jan 31, 2019)

honesttjohn said:


> Check your Safe Z and Home position settings.
> 
> Does the preview show the deep cut?


My Safe Z is set at 0.800
I didn't look to see if the preview shows it. I can check when I get home this afternoon.


----------



## honesttjohn (Feb 17, 2015)

OCEdesigns said:


> My Safe Z is set at 0.800
> I didn't look to see if the preview shows it. I can check when I get home this afternoon.


Your pic shows Safe Z at .2 - not .8


----------



## OCEdesigns (Jan 31, 2019)

honesttjohn said:


> Your pic shows Safe Z at .2 - not .8


You're right. My Home Z is .8 and Safe Z is .2


----------



## beltramidave (Jan 6, 2016)

Is it possible that you forgot to recalculate your toolpath after setting your passes = 3? I have forgotten to do that on occasion after making a toolpath change. You could look at the gcode and see what it is being told to do on the first pass.

I would also recommend ramping instead of plunging to cut depth.


----------



## BalloonEngineer (Mar 27, 2009)

A couple of possibilities. How was the stock held down? If clamped around edge, possibly not flat everywhere or lifting do to upcut. This may be a good application for the blue tape and superglue method.

How did you zero off the top of material? If you use touch off puck, make sure that the thickness is set correctly. Mine seems to have not read some types of bits as consistently, have mine back off to 1", and double check with a 1-2-3 block.

Several sharks that I have seen tend to have a little flex in the gantry do to the unsupported rails, possible that "grabbing" of the aluminum is pulling the entire Z carriage down a slight bit. If you push up or down on the collet, is there any movement?

Do you know the alloy of the aluminum? I have had better luck with harder alloys (6061) than with softer (3003) alloys. The soft ones are gummy and grab more.

When cutting aluminum, I like to lubricate the bit with this spray. Use it all the time, but it seems to make a more noticeable difference with aluminum. May not be as necessary if you were using wd40, I have been cutting dry most of the time (or just air blast).


----------



## OCEdesigns (Jan 31, 2019)

beltramidave said:


> Is it possible that you forgot to recalculate your toolpath after setting your passes = 3? I have forgotten to do that on occasion after making a toolpath change. You could look at the gcode and see what it is being told to do on the first pass.
> 
> I would also recommend ramping instead of plunging to cut depth.


I'm sure it's possible but I even did the test piece and it was set to 3 passes of 0.010 and it also started at 0.035. I would normally ramp instead of straight plunge but since it was supposed to only go 0.010 I didn't think the ramp was as necessary. 

How do I bring up the G code? Can I just open the .tap file in another program?


----------



## OCEdesigns (Jan 31, 2019)

BalloonEngineer said:


> A couple of possibilities. How was the stock held down? If clamped around edge, possibly not flat everywhere or lifting do to upcut. This may be a good application for the blue tape and superglue method. Clamped around edge but had no noticeable lifting
> 
> How did you zero off the top of material? If you use touch off puck, make sure that the thickness is set correctly. Mine seems to have not read some types of bits as consistently, have mine back off to 1", and double check with a 1-2-3 block. I did use the touch plate. I checked calibration a few weeks ago but will check again
> 
> ...


 I can try that spray. I have used WD40 in the past and a friend of mine who is a tool maker with the big CNC stuff also recommended it. But I'm always open to try stuff

Please see the Red responses above.


----------



## kp91 (Sep 10, 2004)

OCEdesigns said:


> I'm sure it's possible but I even did the test piece and it was set to 3 passes of 0.010 and it also started at 0.035. I would normally ramp instead of straight plunge but since it was supposed to only go 0.010 I didn't think the ramp was as necessary.
> 
> How do I bring up the G code? Can I just open the .tap file in another program?


Try opening your g code file in 'notepad'. My post processor uses the extension *.tap and it displays in notepad just fine.


----------



## OCEdesigns (Jan 31, 2019)

kp91 said:


> Try opening your g code file in 'notepad'. My post processor uses the extension *.tap and it displays in notepad just fine.


Doug
Thanks I will try that when I get home today from work. I should have brought the laptop here! lol


----------



## UglySign (Nov 17, 2015)

Try Notepad++


----------



## OCEdesigns (Jan 31, 2019)

UglySign said:


> Try Notepad++


That one looks nice. Thanks for the info!!


----------



## OCEdesigns (Jan 31, 2019)

Here is my G-Code. I don't see any reason for the first pass to be 0.035 deep. I looked at the entire code and it shows what I should be seeing of first pass depth of 0.010. I guess I need to check other places. Hopefully it's the touch plate calibration.


----------



## ger21 (Feb 10, 2019)

Your Z zero is set incorrectly.


----------



## OCEdesigns (Jan 31, 2019)

ger21 said:


> Your Z zero is set incorrectly.


Gerry
I was hoping you would chime in!
Where do you see that it's set incorrectly? What am I missing or what did I set wrong?

The same issue happened on my test piece. But on the original sign the first thing I did was some engraving of 2 words and had no depth issues with the engraving bit and I set the Z zero the same with the touch plate. 

I plan to do some more testing after work today on some wood and also check the calibration of the touch plate.


----------



## ger21 (Feb 10, 2019)

When it's cutting the first pass, what depth is displayed on the DRO on your screen? Is it 0.01, or 0.035?

If it says 0.01, the you set Z zero for that tool incorrectly. If it says 0.035, then the issue is with your control, as the g-code clearly calls for a cut depth of .01.

This should have nothing at all to do with V Carve Pro.


----------



## OCEdesigns (Jan 31, 2019)

ger21 said:


> When it's cutting the first pass, what depth is displayed on the DRO on your screen? Is it 0.01, or 0.035?
> 
> If it says 0.01, the you set Z zero for that tool incorrectly. If it says 0.035, then the issue is with your control, as the g-code clearly calls for a cut depth of .01.
> 
> This should have nothing at all to do with V Carve Pro.


All I have is the pendant controller which does not show any DRO of what is actually happening.


----------



## ger21 (Feb 10, 2019)

After you set Z zero, can you jog the machine to a location where you can verify it's correct, before running the program?


----------



## OCEdesigns (Jan 31, 2019)

ger21 said:


> After you set Z zero, can you jog the machine to a location where you can verify it's correct, before running the program?


Yes I can. This is what I will be trying today after work. 

This might be a stupid question but I was just thinking about it this morning. The touch plate is Aluminum and the material is Aluminum. As I'm setting Z zero can that have any affect on it? The bit is simply completing a circuit when it touches the plate so I don't think it can but thought I would throw it out there!


----------



## ger21 (Feb 10, 2019)

That's how mine works, and it's perfect every time.


----------



## OCEdesigns (Jan 31, 2019)

ger21 said:


> That's how mine works, and it's perfect every time.


Ok cool. After I test a few things I'll update it here.


----------



## TimPa (Jan 4, 2011)

pretty sure the touch pad circuit is through the router/spindle, bit, and touch pad (wire). Whatever material is underneath the touch pad will have no impact, other that its thickness for the Z zero.


----------



## MEBCWD (Jan 14, 2012)

Chad I finally took a break and found your post. The sharks are notorious for bad readings with a touch plate. Get in the habit of watching when the bit touches the pad and now and then you will see it push the pad down a little, this will result in a bad reading so redo your touchplate routine.

Also don't use Virtual Zero on anything critical. It is overrated in my opinion and can cause more problems on some jobs that it is worth. You have to remember that Virtual Zero uses the five reading you take and recalculates your gcode file so if any of those readings are bad it uses them to recalculate the gcode and just builds the error in a file. If you are cutting anything that needs to be good/right on the money, trim a spoil board and don't use Virtual Zero. 

Also hate to say it but the flex in a Shark might be too much for those cut depths.


----------



## tulowd (Jan 24, 2019)

Re WD40 on aluminum

I have used this to clean my Mustang engine bay and all the various alum pieces on my snowmobiles.
Works great, displaces water and is a little bit of a lubricant that displaces water ,so it's great for wiring. It is however, also a mild solvent and leaves behind a film. In my experience it does not harm automotive or snowmobile wiring insulation or connectors, but your experience may differ.

Aluminum being highly porous will absorb it and you will never get it all out, so if you plan on polishing or clear coating/painting it, be prepared, probably to seal it, with no guarantee of success.

Alum comes up quite nice in a brushed/sanded finish and can be satin polished by hand using WD40. I guess I'm saying once it's on/in there, it ain't coming out and could cause some surface treatment issues with fish-eyes, lack of adhesion etc.
Love the look of raw alumimun, I had my old German Borbet Type A wheels polished and used them like that for 20 years on my car.


----------



## OCEdesigns (Jan 31, 2019)

MEBCWD said:


> Chad I finally took a break and found your post. The sharks are notorious for bad readings with a touch plate. Get in the habit of watching when the bit touches the pad and now and then you will see it push the pad down a little, this will result in a bad reading so redo your touchplate routine.
> 
> Also don't use Virtual Zero on anything critical. It is overrated in my opinion and can cause more problems on some jobs that it is worth. You have to remember that Virtual Zero uses the five reading you take and recalculates your gcode file so if any of those readings are bad it uses them to recalculate the gcode and just builds the error in a file. If you are cutting anything that needs to be good/right on the money, trim a spoil board and don't use Virtual Zero.
> 
> Also hate to say it but the flex in a Shark might be too much for those cut depths.


Mike I'm going to say you are right. And after a few suggestions from Gerry I was doing some tests and found a few things. These were not as noticeable on wood but showed up a lot on the aluminum. 
First is my plunge rate with the touch plate was too fast. 10 IPM and causing it to "Push down" on the material too quickly before reading it. I slowed it to 5 IPM then to 2 IPM and at 2 IPM I get much more accurate readings. 
Second which kind of relates to the first is the inherent flex in the spindle mount / Gantry also contributed to the depth issues. 
Now I tested the touch plate about 15 times at the 2 IPM. Each time I used the touch plate in different areas and then checked it's accuracy manually with a piece of paper and now each time it is very close to zero. Within 1 to 3 thousands. I then ran another test run on aluminum. First pass was set to 0.010 and actually cut that!! I ran a set total depth of 0.030 and ended up with 0.036. For using a machine designed for wood and getting that close on Aluminum I'm pretty happy now. 
I was really hoping to not use a spoil board because I use my clamps in a lot of different ways. I may need to look into it more and get creative on the board for for my clamping needs. 
Thanks again for all the responses and ideas. Not sure it's 100% figured out but I now know I'm much better!!


----------



## OCEdesigns (Jan 31, 2019)

tulowd said:


> Re WD40 on aluminum
> 
> I have used this to clean my Mustang engine bay and all the various alum pieces on my snowmobiles.
> Works great, displaces water and is a little bit of a lubricant that dissipates. It is however also a mild solvent and leaves behind a film.
> ...


Paul
Thanks for the info! I also like the raw Aluminum look too.


----------



## radios (Sep 30, 2009)

you need to do climb milling on Aluminum!. else you get rough cuts..


----------



## OCEdesigns (Jan 31, 2019)

radios said:


> you need to do climb milling on Aluminum!. else you get rough cuts..


Maybe a stupid question but why does it matter? I'll check my program because I think I had it set to Conventional. In wood I know I get different "Smoothness" on the finishes with Climb and Conventional.


----------



## radios (Sep 30, 2009)

OCEdesigns said:


> Maybe a stupid question but why does it matter? I'll check my program because I think I had it set to Conventional. In wood I know I get different "Smoothness" on the finishes with Climb and Conventional.


Aluminum is soft and sticky when cut, climb milling prevents the rough cut that you would get with conventional milling on Aluminum. I've milled and turned many thousands of pieces of Aluminum..


----------



## OCEdesigns (Jan 31, 2019)

radios said:


> Aluminum is soft and sticky when cut, climb milling prevents the rough cut that you would get with conventional milling on Aluminum. I've milled and turned many thousands of pieces of Aluminum..



Thanks Martin!


----------

