|
Post by Derek the Admin on Aug 14, 2017 20:17:50 GMT
What was the intent of the run? Looks like you it didn't get setup to go any deeper?
The motors aren't damaged. They just stalled which sounds bad but isn't that big of a deal. Every CNC operator has stalled them.
|
|
|
Post by VGCustomShop on Aug 14, 2017 23:00:16 GMT
Thanks for the reply - what happened is frustrated trying to program the gcode in fusion - I made the model with the y axis up - and should've made the model with the z axis up - anyway - although the simulations all look good the gcode will not make it past post processing without failing. So I asked a friend to make me some gcode - the video is what happened after using his code - which is made for mastercam and a diferent machine. I'm back to working on the gcode in fusion - watched the video you sent on coordinates - but am still not having any luck. Will keep trying. Update: finally got the gcode - now for a test . . . wish me luck. Woops - I don't know where to tell the router to start - don't know where to put my stock . . .
|
|
|
Post by Derek the Admin on Aug 14, 2017 23:05:03 GMT
What specific errors is it giving you when you try to post process?
The model orientation shouldn't mess you up since you can change it. Are you able to change the CAM orientation as shown in the video or is that failing?
Can you share the Fusion project so one of us could take a look at the the project itself?
|
|
|
Post by VGCustomShop on Aug 14, 2017 23:33:00 GMT
What specific errors is it giving you when you try to post process? The model orientation shouldn't mess you up since you can change it. Are you able to change the CAM orientation as shown in the video or is that failing? Can you share the Fusion project so one of us could take a look at the the project itself? a360.co/2uWeMeCI have the code now - after watching the video you suggested was able to orient the work - now I need to think about where zero and the wood should be . . .
|
|
|
Post by Derek the Admin on Aug 15, 2017 13:13:07 GMT
I just looked at your f3d file and your CAM settings. It looks like you have Z properly set now. Here are a few observations that will help you be successful: ADAPTIVE CLEARING: It is set up to cut too slow and too deep. Your cut depth is 0.393. With that's a 10mm deep cut and it's too much. Your feed is a bit to slow, resulting in an inadequate chipload. I don't know your exact materials and I don't use such a long endmill (I realize it is necessary for what you are doing), so it's hard for me to give you exact settings, but if I were you I'd set my cut depth to more like 0.15 or even 0.125 inch and up my feed rate to about 85 or 90 IPM. The operation will take about as long and you will be pulling out a chip large enough to keep the endmill cooler, which will make it last longer. Eventually, a dulled end mill is like trying to run a spinning spoon through the wood. CONTOUR: I think here you should also speed it up to about 85 or 90IPM. I feel like you can increase your step down as well from the 0.04" it is set to now. Let the machine be your guide there though because as I said I'm not accustomed to such a long end mill, which creates quite a long lever arm. I would also look into roughing and finishing passes if I were you. This will do two things for you. First, it will allow a little skim pass on the outer body of the guitar to remove some of the tooling marks that would otherwise require (more) sanding to finish smooth. Secondly, it will give the wood chips a place to go. The cutter is going to be very deep into that stock and a slot just equal to the diameter of the end mill provides very little room for the chips to evacuate, plus it's essentially cutting on both sides of the tool, increasing the forces upon it. This is often more a concern in metal, but as deep as you are I'd consider doing it. Plus it will come off the machine smoother with a finishing pass. Also, I'd look at tabbing it in some places. It's a big piece, so it is less likely to move, but you will be very upset when an hour or so of running ends in the work piece shifting and getting slammed into the end mill, ruining the guitar body.
RAMP: I don't use this operation much. I see exactly what you are doing and I don't have any objections here except for the feed rate needing to be increased some and putting it before the contour operation. You may also want to consider a point cutting round over bit. A ballnose can do it, but I like to machine a constant geometrical feature (such as that edge radius) with tools matched to the geometry. Really though, if I were doing this, despite having a CNC company and a CNC shop.... I'd pull it off and round it over on a router table manually. I say this because you can't machine the face down side anyway and will have to run it manually I'm sure. Running both sides manually will allow you to achieve the same exact same radii on both sides. I don't know much about guitars so that may not be the standard, I'm just assuming.
All that said, test the settings I proposed on scrap pieces first please. I don't want you to dive in on my advice and ruin a piece.
|
|
|
Post by VGCustomShop on Aug 16, 2017 10:51:15 GMT
I just looked at your f3d file and your CAM settings. It looks like you have Z properly set now. Here are a few observations that will help you be successful: ADAPTIVE CLEARING: It is set up to cut too slow and too deep. Your cut depth is 0.393. With that's a 10mm deep cut and it's too much. Your feed is a bit to slow, resulting in an inadequate chipload. I don't know your exact materials and I don't use such a long endmill (I realize it is necessary for what you are doing), so it's hard for me to give you exact settings, but if I were you I'd set my cut depth to more like 0.15 or even 0.125 inch and up my feed rate to about 85 or 90 IPM. The operation will take about as long and you will be pulling out a chip large enough to keep the endmill cooler, which will make it last longer. Eventually, a dulled end mill is like trying to run a spinning spoon through the wood. CONTOUR: I think here you should also speed it up to about 85 or 90IPM. I feel like you can increase your step down as well from the 0.04" it is set to now. Let the machine be your guide there though because as I said I'm not accustomed to such a long end mill, which creates quite a long lever arm. I would also look into roughing and finishing passes if I were you. This will do two things for you. First, it will allow a little skim pass on the outer body of the guitar to remove some of the tooling marks that would otherwise require (more) sanding to finish smooth. Secondly, it will give the wood chips a place to go. The cutter is going to be very deep into that stock and a slot just equal to the diameter of the end mill provides very little room for the chips to evacuate, plus it's essentially cutting on both sides of the tool, increasing the forces upon it. This is often more a concern in metal, but as deep as you are I'd consider doing it. Plus it will come off the machine smoother with a finishing pass. Also, I'd look at tabbing it in some places. It's a big piece, so it is less likely to move, but you will be very upset when an hour or so of running ends in the work piece shifting and getting slammed into the end mill, ruining the guitar body. RAMP: I don't use this operation much. I see exactly what you are doing and I don't have any objections here except for the feed rate needing to be increased some and putting it before the contour operation. You may also want to consider a point cutting round over bit. A ballnose can do it, but I like to machine a constant geometrical feature (such as that edge radius) with tools matched to the geometry. Really though, if I were doing this, despite having a CNC company and a CNC shop.... I'd pull it off and round it over on a router table manually. I say this because you can't machine the face down side anyway and will have to run it manually I'm sure. Running both sides manually will allow you to achieve the same exact same radii on both sides. I don't know much about guitars so that may not be the standard, I'm just assuming. All that said, test the settings I proposed on scrap pieces first please. I don't want you to dive in on my advice and ruin a piece. Many thanks for the help Derek - Followed all of your suggestions and the machine is running beautifully. Here's what is the issue now - either the controller, the gcode or the gcode sender are not working correctly. On 4 occasions the program froze before tasks were complete. Another time the machine ran the mill across a place it wasn't supposed to after doing several correct passes. Another time the machine started to rout the neck pocket correctly except it was raising too high between passes - then it continued routing the pocket past an inch deep (it's supposed to be 5/8") so the program had to be stopped. So far the machine has never been completely through a cycle or task without a glitch. Also switched to my better laptop - but the same types of things still happened. On a marginally brighter note - it almost made it through a cycle when a clamp came loose. That said - it's not reliable. Any ideas? Oh and BTW - my computer is plugged in and set to always on - it was working fine when the UGCS froze. Also, am totally hip to roundovers etc. I have a table router, overarm router and two neck jigs with routers mounted - and typically will not use the CNC to do profiles or round overs - just experimenting to get used to the machine. It will hopefully do arm and belly contours and arched tops when my modeling skills get there.
|
|
|
Post by Derek the Admin on Aug 16, 2017 13:49:06 GMT
Happy to help. Very doubtful it's the controller or g code. This is a computer or g code sender issue. I'd suggest some dry runs on some things using different G Code senders. As I understand it, UGS makes different copies of the g code and tracks each as it goes through I've not had any problems with UGS Platform but you might also want to try Grbl Panel or kiri moto (I don't use kiri motor at all). I'll emphasize that you need to just do dry runs on this while that's sorted out. Then there's PicSender by the PicEngrave people. It's 25 bucks but advertised as being a super efficient g code sender. I have it and it always runs very smoothly. I use it to run laser picture engraving files that are very intensive. I don't recommend it though because the jogging controls are pretty glitchy it seems.
|
|
|
Post by aforww on Aug 16, 2017 14:58:01 GMT
Maybe power issues? I know mine was doing some weird stuff. Pausing briefly but the code continued to run so when it picked back up the bit was in the spot it stopped but the code had continued on so screwed up everything. I found that the power supply was actually cutting off momentarily. The same could happen if there are spikes as power loss. Something to look at. Might also check USB. Maybe a bad cord?
|
|
|
Post by VGCustomShop on Aug 20, 2017 11:34:48 GMT
Happy to help. Very doubtful it's the controller or g code. This is a computer or g code sender issue. I'd suggest some dry runs on some things using different G Code senders. As I understand it, UGS makes different copies of the g code and tracks each as it goes through I've not had any problems with UGS Platform but you might also want to try Grbl Panel or kiri moto (I don't use kiri motor at all). I'll emphasize that you need to just do dry runs on this while that's sorted out. Then there's PicSender by the PicEngrave people. It's 25 bucks but advertised as being a super efficient g code sender. I have it and it always runs very smoothly. I use it to run laser picture engraving files that are very intensive. I don't recommend it though because the jogging controls are pretty glitchy it seems. On my last nut - UGCS will not complete a file without freezing - Source Rabbit finishes but changes the shape of the routes, picsender wont work at all because it says that the gcode is in error and no matter how many times 0 is set the program says 0 may have been lost and that the gcode has an error that MAY be on or before line 3 - but don't know what to look for and it seems to work in other programs - not sure what to do. So the only way to route a guitar is to separate all the pockets into groups of two - or one file for two pockets - it seems UGCS does fine for three pockets and sometimes three. So far only managed to ruin a bunch of cheap wood. LOL - really frustrated. Interestingly, building the machine was fairly simple, learning Fusion isn't too bad either - getting the gcode and or sender software working correctly is a real grizzly bear.
|
|
|
Post by Derek the Admin on Aug 20, 2017 14:12:42 GMT
My best advice would be to file a support request on the Universal G Code Sender GitHub or with PicEngrave. They may know something about their program that we don't. I truly wish I could be more helpful in this respect but I have not encountered these issues before.
While splitting the g code into two files and putting half the ops in one and the other have in the second is not the ideal case, it does seem to be a viable work around until you can get the sender program authors to iron out those wrinkles with you.
|
|
|
Post by aforww on Aug 20, 2017 15:38:16 GMT
Can you share the Fusion file and gcode so I can look at it? There's obviously something wrong with the Gcode or the way it was designed.
|
|
|
Post by VGCustomShop on Aug 20, 2017 22:10:48 GMT
My best advice would be to file a support request on the Universal G Code Sender GitHub or with PicEngrave. They may know something about their program that we don't. I truly wish I could be more helpful in this respect but I have not encountered these issues before. While splitting the g code into two files and putting half the ops in one and the other have in the second is not the ideal case, it does seem to be a viable work around until you can get the sender program authors to iron out those wrinkles with you. Excellent advice! John at Picsender has this to say about the code produced by Fusion: ". . . The .nc file you sent needs the % removed from the beginning and end of the file. That is used in Mach3 to ignore the comments. The T22 M6 needs to be removed also. GRBL does not support tool change commands. Since the file attached is a Vector file, the Vector Gcode needs to be selected in PicSender." It apparently worked fine for the guy at picsender after that - so looking forward to trying it!
|
|
|
Post by VGCustomShop on Aug 20, 2017 22:13:10 GMT
Can you share the Fusion file and gcode so I can look at it? There's obviously something wrong with the Gcode or the way it was designed. Had a couple folks look at the code - the owner at Picengrave had this to say about the code: " . . .The .nc file you sent needs the % removed from the beginning and end of the file. That is used in Mach3 to ignore the comments. The T22 M6 needs to be removed also. GRBL does not support tool change commands. Since the file attached is a Vector file, the Vector Gcode needs to be selected in PicSender." He said it worked fine on his machine once these changes were made.
|
|
|
Post by aforww on Aug 20, 2017 22:31:12 GMT
Excellent, glad you got it worked out! Gotta watch files you get from other sources. Especially if they don't tell you what was used to make it and what they use to run it. Commands like M0,M1, coordinates, offsets, ignore commands, can really ruin your day.
|
|
|
Post by VGCustomShop on Aug 21, 2017 5:37:51 GMT
Excellent, glad you got it worked out! Gotta watch files you get from other sources. Especially if they don't tell you what was used to make it and what they use to run it. Commands like M0,M1, coordinates, offsets, ignore commands, can really ruin your day. The code was generated by Fusion 360 by selecting generic grbl in the post processor after making the model.
|
|