Tool not lifting to clear material

[ROBERTHAIGHT1851]

When I run a setup to cut a 2D contour, the heights seem to be okay, but the machine doesn't lift above the material at the beginning or end and just plows through the piece. (Cutting 3/4" ply if that matters. Even when I set the Feed Height and others to ridiculous numbers like 3 inches, it does the cuts and goes way up and way down between passes, but it still drops 3/8" below the top of stock when it first starts and when it finishes and goes to its end point.

Been checking things like Safe Distance (.28937).

I haven't run this in a while, but have made numerous parts before and this is a first.

Any help will be appreciated

[engineguy]

@ROBERTHAIGHT1851 

Without a file it is very hard to diagnose if you have a setting wrong somewhere, to upload a Fusion f3d file go to :-

File > Export > Select f3d format > Save to your computer and then attach to your reply.

I suspect that it might be how you have setup at your CNC, from reading your post it sounds like the machine is lifting up to the clearance heights when moving from one cut to the next that you are setting in Fusion so the code sounds correct, if you don`t have your CNC and tools set correctly then what you describe is most likely 🙂

[programming2C78B]

Do you have g28 home enabled? Ensure machine g53 z0 is actually at the top of your machine limits before starting. Common issue with hobbyist machines.

[ROBERTHAIGHT1851]

I wish I knew.  I looked at some of the post processed files I created and have been using and don't see G28 in the area where I think it should be.

I looked at the Post Processing setting screen and can see it says Safe Retracts G53

I spent much of yesterday trying to be certain I had the latest Onefinity drivers and post processor related to the machine

[engineguy]

@ROBERTHAIGHT1851 

The codes G28 G91 Z0 and G53 G0 Z0 do the same thing, it depends on what the CNC Control is configured to accept.

However they can only work correctly if the CNC Control has been setup to go to the Machine "Home" position, usually machines have Limit switches that are used for both the "Home" position and machine overrun.

If the machine does not have actual switches to home to then you need to use a safe position by jogging the machine in the X/Y/Z and setting that position as your machines "Home" position, this means that if either of the G53 or G28 command lines are in the code your machine will go to that preset position every time.

If you don`t want this to happen then you can use the "Clearance Height" option, if you use this option then you will not get any G53 or G28 command lines posted anywhere in the code.

This means that great care must be taken when setting up your Part Zero position at the machine as you now have no safety/Home positions.

Your actual Clearance height will depend on how you set your Heights for the operation, for example see the image below, those settings will produce a total Clearance height of 25mm because the WCS has been set to the Bottom corner so the Clearance is calculated from there. If I move the WCS to the Top of the Stock then the Clearance will be calculated from that point and the total Clearance will be 20mm with the same Height settings.

So, as you can see great care needs to be used if using just the "Clearance Height", I know that many folks like to work that way so they don`t have a lot of wasted time with the Machine keep going all the way up to it`s Z home position.

WCS at bottom Clearance 25mm

WCS at Top Clearance 20mm

Nothing wrong with this method but it does need a little more care when setting up at the machine 🙂 🙂

So, just a matter of matching things up at the CNC and Fusion 🙂 🙂 Hope this isn`t too confusing and helps a little 🙂 🙂

[ROBERTHAIGHT1851]

This is so helpful. Thanks for taking the time.  I am pretty certain that my issue is in this area somewhere.

When I look at the Gcode there is a line

N20 G53 G0 Z0

Could that be saying that the z height is 0 (zero)?  Wouldn't that be a problem?

Thanks again

[engineguy]

@ROBERTHAIGHT1851 

That G53 G0 Z0 is the Command line that should send the CNC to the Z axis "Home" position, it is not the Z Zero position of your Stock.

There are two Z0 positions at a CNC Machine and are often confused, one is the Machine Z0 position and the other is the Part Z0 which is normally set at the top of the Stock, the Machine Z0 is usually the highest point of the Z axis travel.

You need to read the Manual for your CNC Control to learn how to set the CNC to it`s Home position usining either physical switches on the machine or if there are none the how to set what are known as "Soft Limits" and how to set a safe "Home" position.

Then once that is all done you can place a piece of stock on the machine and "Touch Off" say for example the top of the stock at the left corner closest to you when facing the machine, that point will be your X/Y/Z Part Zero, the numbers on your read out should then be input to the G54 in your Fixtures Table, that then tells the Control exactly where the corner of the stock is on the Table.

Now, if you use that position at the CNC then you need to use the same position on your stock in Fusion so that the X/Y/Z coordinates generated by Fusion will be moved by the G54 command to the correct position at your CNC.

Again, there are two Z0 positions at your CNC, one for the Part Z0 and one for your CNC Machine Z0, do not set the CNC Machine Z0 to the Stock or to the Table, if it is set to the Table then the machine will go straight to that point when it sees a G53 G0 Z0 command and likely go through your stock at full speed to get there !! Ouch !! 😞 😞