|
Post by scottacus on Nov 29, 2018 2:19:25 GMT
I'm just making my first cuts with code that I generated in Fusion 360 and had a few questions about the process 1) It seems that the code will error in the Universal GCode Platform if I don't remove the lines that contain M code at the top of the Gcode is this normal? M9 T1 M6 S24000 M3 2) The Fusion 360 inserted this at the end which caused the mill to cut into the side of the contour when it lifted out : G1 X55.08G0 Z15 Is this something that I accidentally inserted ? 3) When I removed the G1 X55.08 the mill exited the contour but still leaves a little nick in the outboard edge of the contour, do I need to make any adjustments to the gantry or is this normal? Here is a photo of some of the profiles that I cut, you can see the big nick in the middle top one from G1 X55.08 and small nicks in the other to the right side.
|
|
|
Post by Derek the Admin on Nov 29, 2018 3:41:41 GMT
You are correct about the M6 code. You can also use the expression remover on UGS to ignore any instance of it in the code. It’s just warning you that it sees a tool change command.
I’m not sure about the X move prior to lifting. That is just weird.
The nick you are seeing is because Fusion thinks you want to cut that square that’s left to the interior. It sees that as the part and assumes you don’t care about what is around it. Fusion kind of assumes you have a block of material in a vise that you are machining away to a final shape (the model, in this case the cube you designed). You could possibly get rid of that by removing lead in and lead out moves.
|
|
|
Post by scottacus on Nov 29, 2018 4:04:51 GMT
Thanks for the quick reply! Since I'm just getting started I wanted to make sure that my machine is operating as expected. I assume the extra motion code is something that I must have mucked up.
When you choose ramping, as in your video, does the machine just ramp until it gets to a set depth, complete the circuit and then ramp down again or does it constantly ramp it's pass continuously? If it has a constant ramp, how do you keep from having really deep cuts if the path around the contour is very long?
Thanks for a great product!
|
|
|
Post by James@fireaxe on Nov 29, 2018 5:19:52 GMT
When I post process from F360, I make a few edits.
%
(1001)
(T40 D=3.14 CR=0 - ZMIN=-18 - flat end mill)
G90 G94
G17
G21
G91 Z10 <--- Delete "G28" add "Z10"
G90
(2D Contour1)
M9
T40 M6 <-- Delete entire Line tool change code, UGS doesn't like it and throws a code each time, so I just delete it.
S26000 M3
G0 Z10 <---- Delete "G54" and add "G0 Z10"
M8
G0 X140.27 Y311.137
Z15
Z5
G1 Z3 F333.3
Z2.5
X140.306 Y311.102 Z2.498 F333
X140.607 Y310.802 Z2.483
X140......
.... LOTS OF CODE!
X-171.352 Y143.299
X-171.675 Y144.349
G0 Z15
M9
G28 G91 Z0 <-- Delete line
G90 <--- Delete line
G28 G91 X0 Y0 <---Delete line
G90
M30
%
I make these edits on each one of my process G code files with Brackets. My machine was trying to home each time I had a G28 code, so I just take them out. Havent had a problem since.
As far as the Ramping operation for a 2D contour, the machine will ramp until it reaches your set depth per pass and when it completes the pass it will ramp again until the it reaches your set depth per pass again.. and will repeat this until it reaches the very bottom depth of your model.
Hope this helps. Happy Carving.
|
|
|
Post by scottacus on Nov 29, 2018 14:06:25 GMT
Thanks for the detailed help! I saw in the excellent intro video on the MillRight site that in Fusion 360 you can turn G28 off in the Post Process Properties section.
BTW I really like the many different signs and carvings that you've posted on the Projects section of the forum. What program are you using to generate the Gcode for these?
|
|
|
Post by James@fireaxe on Nov 29, 2018 14:57:48 GMT
Thanks for the detailed help! I saw in the excellent intro video on the MillRight site that in Fusion 360 you can turn G28 off in the Post Process Properties section. BTW I really like the many different signs and carvings that you've posted on the Projects section of the forum. What program are you using to generate the Gcode for these? I use F360 for all my modeling and the internal CAM program inside F360 (tool paths that generate G code) programs. I use Universal G Code Sender to send the code to the machine.
|
|
|
Post by tjstandley on Nov 29, 2018 16:41:29 GMT
Check your Lead-In and Lead-Out settings in Fusion 360 - I think you are seeing a lead out problem. You can adjust the settings (such as angle) or you can just uncheck the box next to it in this case.
|
|
|
Post by Big Man Black T-Shirt(Patrick) on Dec 2, 2018 22:16:58 GMT
When I post process from F360, I make a few edits. (2D Contour1) M9 T40 M6 <-- Delete entire Line tool change code, UGS doesn't like it and throws a code each time, so I just delete it.HA! I do a similar thing with each of my F360 docs. I remove a T3 M6 and put a "Z10" in its place.
|
|
|
Post by jamesterm on Dec 3, 2018 15:36:11 GMT
When I post process from F360, I make a few edits. T40 M6 <-- Delete entire Line tool change code, UGS doesn't like it and throws a code each time, so I just delete it.
I use HsM Express and all I do is take out the M6 (Using same UGS of course). I agree and should do the same with the G28's but I don't understand the benefit of deleting G54, can you tell me why this needs to be deleted? For reference: HsM Express should be very similar to F360... here's a sample of an unedited header and footer Note, I use inches: (2D Contour3) G90 G94 G17 G20 G28 G91 Z0 G90 (2D Contour3) M9 T1 M6 (for hard Aluminum) S19666 M3 G54 G0 X1.8509 Y-1.9159 Z0.6 G0 Z0.2 X-1.891 Y1.877 .... lots of code.... G0 Z0.6 G28 G91 Z0 G90 G28 G91 X0 Y0 G90 M30
|
|
|
Post by James@fireaxe on Dec 3, 2018 15:49:05 GMT
When I post process from F360, I make a few edits. T40 M6 <-- Delete entire Line tool change code, UGS doesn't like it and throws a code each time, so I just delete it.
I use HsM Express and all I do is take out the M6 (Using same UGS of course). I agree and should do the same with the G28's but I don't understand the benefit of deleting G54, can you tell me why this needs to be deleted? For reference: HsM Express should be very similar to F360... here's a sample of an unedited header and footer Note, I use inches: (2D Contour3) G90 G94 G17 G20 G28 G91 Z0 G90 (2D Contour3) M9 T1 M6 (for hard Aluminum) S19666 M3 G54 G0 X1.8509 Y-1.9159 Z0.6 G0 Z0.2 X-1.891 Y1.877 .... lots of code.... G0 Z0.6 G28 G91 Z0 G90 G28 G91 X0 Y0 G90 M30 It was in one of the videos Derek posted for beginners. G54-G59 is used for multiple work ordinate systems if you are working on multiple pieces on the same bed. I believe since Im using just one WCS, there is no need for the G54 code so instead, a G0 (rapid move) Z10 is set to move the bit an additional 10mm above stock. As advised by Derek, all my measurements are in MM. This was also in the video. If it doesnt affect your machine with it left alone, then I say leave it. I just have developed a habit of taking it out and have had no issues since. Hope this helps. James
|
|
|
Post by jamesterm on Dec 3, 2018 16:33:46 GMT
It was in one of the videos Derek posted for beginners. G54-G59 is used for multiple work ordinate systems if you are working on multiple pieces on the same bed. I believe since Im using just one WCS, there is no need for the G54 code so instead, a G0 (rapid move) Z10 is set to move the bit an additional 10mm above stock. As advised by Derek, all my measurements are in MM. This was also in the video. If it doesnt affect your machine with it left alone, then I say leave it. I just have developed a habit of taking it out and have had no issues since. Hope this helps. James I see... I went ahead and researched this a bit and fount this link <-link->They (F360/HsM) add it... as it is understood to be zero'd (and remain zero'd) as a way to have a clean exit from a previous session. I believe $h also ensures this is cleared (or it may just start up that way I'll have to check)... I can see the benefit or removing this, if somehow it starts up uninitialized, and it serves no benefit to keep if we work with one WCS (I do as well). Thanks for explanation.
|
|
|
Post by joebob296 on Dec 4, 2018 5:07:05 GMT
Just curious, but do you guys have to manually edit all these changes everytime? Or can you set it to automatically do this?
|
|
|
Post by Big Man Black T-Shirt(Patrick) on Dec 4, 2018 9:46:36 GMT
Just curious, but do you guys have to manually edit all these changes everytime? Or can you set it to automatically do this? I'll be honest, I just fell into the habit when the Tx Mx line gave me problems and just never followed through to find a permanent solution. Now it's almost automatic, i post, open it in TextWrangler, replace with Z10, look over everything, Save, and move on. It's on my list of things to do "someday" to make it a permanent, automatic fix. But like John Fogerty said, "someday...never comes..."
|
|
|
Post by James@fireaxe on Dec 4, 2018 11:17:54 GMT
Just curious, but do you guys have to manually edit all these changes everytime? Or can you set it to automatically do this? I haven't found a fix to remove the G28 and the T code, so I do it every time. Mostly I haven't even investigated it, so it's more Just a habit I have developed. I actually don't mind doing it at all.
|
|
|
Post by jamesterm on Dec 4, 2018 14:07:15 GMT
Just curious, but do you guys have to manually edit all these changes everytime? Or can you set it to automatically do this? You have given me an idea... if enough people are willing to use a command prompt I can add it to my gcode tool program. What this software does is it can make your CNC machine to play music, and provides tab support (since HsM Express doesn't have it). I can add a new command to auto fix these edits. If this is something anyone would like to try let me know. This software as it currently stands is here: <--GCodeTools.zip-->
|
|