You are going off the rails here guy. First, if you pick up the edge of the part using the edge of the tool then in Mach you need to zero the axis then add the tool radius to the DRO if you are on the plus side or subtract if on the minus side. In MDI if you are in absolute mode and type X0 Y0 your tool should center on 0,0 and the center of the tool should be on the edge as it should.
Next you have to tell either the CAM program or Mach but not both, the tool diameter in the tool table. If you do this in CAM the g-code will be offset by the tool radius. For an outside profile the g-code will be bigger than the part.  If you want to enter the tool diameter in Mach then you must set the CAM program to output G41/G42 tool radius compensation. Then in Mach you must set up the tool radius in the tool table.
Do yourself a favor for now put the tool diameter in the CAM program until you have more experience. If you are hand programming G41/G42 are your friend. For CAM they will drive you nucking futz.

You can enter them either directly into the Fixture Offsets table (View menu) or via the Diagnostics tab. See the Operations manual for a brief description of their effect.

Allan

Gary

The tool diameter is in the CAM program (Fusion 360), Ive had it in from the start but it appears to have no effect.

I then tried putting the X & Y Offsets in the Mach4 tool table, What appears in the DRO under Tool Offset is the Diameter. see image, Tool 1 is selected, DRO shows Dia Offset as per Dia entered in Mach4 Tool Table.

You can enter them either directly into the Fixture Offsets table (View menu) or via the Diagnostics tab. See the Operations manual for a brief description of their effect.

Allan

The Operations Manual images does not match whats in my version of Mach4 see images.

dq828

Your lower image appears correct, but I'm not seeing their relevance.  You need to look at paragraph
3.5 on Fixture Offsets.

Just go to the Diagnostics tab, enter your cutter radius into the Work Shift fields for X and Y, and see if it does what you want. You may need to experiment with the signs depending where you touch off on the work.

Allan

After mulling this over in the shower, I don't think that the Work Shift would satisfy your need, as I think it would be nullifies each time you subsequently touched off.

So if you cannot move your work zero within the CAM program, why not just do the obvious and set your X and Y  DROs to your tool radius instead of zeroing them at touchoff. For example if you touch off at the south west corner of your stock using  a 10mm cutter, you would set each DRO to -5.0

Allan

Allan

Thanks for the advice, I'll give it a go as soon as I can.

Thanks Again
David

Try this.  Create a 1" square object in Fusion 360.  Select a tool and create the G-code for an outside profile. Look at the G-code.  Is there a G40 output?  Are there radiuses programmed?  If so then the tool radius IS being used.  Are the straight lines equal to 1"?  Are the radiuses equal to the tool radius?  If this is all true then Fusion is doing everything correctly and is using the tool radius.

You need to learn to read G-code a bit.  Fortunately the easiest way is to look at the output from a CAM program.  I use CamBam but I always use Single Block to start a program for the first time, reading each line of G-Code and looking at the DROs to make sure the NEXT operation or move is going to be safe.  When the tool goes where it is supposed to be and the next operation will start cutting I turn off Single Block and let it go with the feed rate turned way down.  Once it is cutting properly I turn the feed rate up.

Little trick.  Always set the feed rate high and turn down the override a lot.  You can turn down way more percentage wise than you can turn the speed up.  I don't like needing the stop and change the program when I find out I can go a lot faster.  You might say you don't need to go faster.  Feeding slow actually wears out tools faster because they are taking more cuts for the same material removal and thin chips cause the tool to skid on the surface work hardening it and dull the tool.  I once adjusted a slotting job in steel that had gone through four end mills already and was only half way done.  I broke two more quickly ,b y turning the speed up.  Then I hit the sweet spot and finished the job on the same end mill.

Gary

Sorry it's taken so long to get back to you, building the CNC wasn't as much of a challenge as I expected, but working out how to use it, with all the different software, and the different settings is turning out to be MUCH more of a challenge than I expected!!!

From what I have been able to acertain Fusion is making allowances directly within the XY coordinates to allow for the cutter size, in other words it's adding and subtracting mm as required. As long as I put the origin where the center of the cutter will be when I set it up in the machine it all seems to work fine.

What I have realised about using a CNC is there are SO many places that you can make an error you (I) have to be very careful at every step, I'm already sick of making mistakes already which I'm normally ok with

Many thanks

While I was testing the offsets I found another issue which I have posted WONKY CUTTING