Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: dq828 on June 02, 2017, 01:42:16 AM
-
I must be missng somethig obvious!
I want to setup my tool (say 10mm Endmill) so that I set the edge of the tool on the edge of the timber I am going to cut (X & Y) but when I do this the program thinks I have set the center of the tool on the edge of the timber so my cuts are 1/2 the diameter out of place. I have played around (and around) with the offset setting in Fusion 360 and Mach 4 but nothing changes.
Can anyone enlighten me as to what I'm doing wrong?
-
do you use G41/G42 or G40?
-
Yes fusion puts a G40 in near the start of the code, I removed it & it made no difference.
I tried a D1 above the T1 as well as removing the G40, nothing. I have shown below the code I have been testing with the Fusion exports.
(17-06-02 V4 OFFSET TEST 9.52MM BIT)
(FEED RATE 1200-200-150- 9.52MM BIT NO TOOL OR OFFSET IN FUSION)
(T0 D=9.52 CR=0. - ZMIN=-4. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90
(2D CONTOUR1)
M5
M9
T0 M6
S10000 M3
G54
M9
G0 X50.24 Y50.
G43 Z45. H0
Z5.
G1 Z2. F200.
Z-1.
G3 X49.76 I-0.24 J0. F1200.
X50.24 I0.24 J0.
G1 Z-2. F150.
G3 X49.76 I-0.24 J0. F1200.
X50.24 I0.24 J0.
G1 Z-3. F150.
G3 X49.76 I-0.24 J0. F1200.
X50.24 I0.24 J0.
G1 Z-4. F150.
G3 X49.76 I-0.24 J0. F1200.
X50.24 I0.24 J0.
G0 Z45.
M9
G28 G91 Z0.
G28 X0. Y0.
M30
-
Hi,
G40 is ok and quite "normal" when using CAM.
If you then run into differences between distances from CAD and distances in real you have to check your tool definitions in the CAM!
G40 means no tool corrections. So the CAM has to calculate the real tool path and for so has to know the exact tool dimensions.
The tool definitions from mach don't come into play with G40.
That means, if you tell your CAM, your tool diameter is 10mm and in real u use a tool with 8mm then you're 1mm off the path (2mm in distance).
Hth Reinhard
-
It's a fusion 360 problem you have the boundary set wrong need it to be on the correct side look at the red arrow on the tool path in the geometry tab flip it over and the tool goes ether inside or out side , e.g. Outside contoured or pocket
There is another setting about tool centre on boundary
I would recommend you post on the fusion forum make sure you post the fd3 file they will sort you out
-
Stuart, thanks but I dont think that is the answer. Im sure I'm being retarded and have missed something simple which I'll try and explan in my next post.
-
I setup my physical tool position against the edges of the piece of wood I’m going to cut, as shown in the Tool Setup image (I do both x & Y like this), this means the center of the tool is setup half the diameter (offset) from the edge of the wood.
I assumed there was an easy way to compensate for this offset in Mach4 (or Fusion 360) but I have not been able to work it out.
My workaround is, with every drawing I do I in F360, I sketch lines offset ½ the tool diameter and setup on that intersecting point as shown in the Fusion Setup images, but this is obviously not the best way to go about it, but it’s the only way I’ve worked out. When I do this everything cuts fine.
I don’t want to have to play with the code that Fusion outputs to achieve my desirable outcome, I would have thought I could set up my physical tool as per the Tool Setup image, and then setup Fusion so the Origin is on the corner of the stock, and either Fusion, or Mach4 would compensate for the different diameter tools.
Eventually I found the Tool Offsets in the Mach4 Tool Table and thought my troubles were over, see Tool Table images to see what I setup.
Well was I wrong, when I ran some test code to Bore a hole, the code that came out of F360 looked ok, but when I tried to run it through Mach4, with F360 set for Tool 3, and Mach4 selecting Tool 3 from its Tool Table, things went haywire.
I didn’t notice the wacky toolpath that Mach4 created at first, but when I tried to actually do the cut, not only did it try to follow the wacko toolpath, but it made my Y axis motors trip out! This happened several times before I noticed the crazy tool path, see image Wacko toolpath 2 image.
When I reverted to Tool 6 which has no setup in the Mach4 Tool Table, the toolpath was fine, the cut was fine, and the motors where fine , see Tool 6 image.
Can anyone tell me how to sort this out?
-
I had issues getting the images to load hence the spread
-
I haven't used them myself, but would Work Shifts give you a way to correct this?
Allan
-
Thanks, where do Work Shifts live? :)
-
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 :)