Printable View
On another note, I did make a sample profiling program to check cutter comp. The output from the post didn't look right from what I've found works on my machine. Unfortunately I don't have time to get into it deeper right now with examples, but will try to get back later today or over the weekend.
Out of curiosity what DX32 software version do you run?
I haven't tested the cutter comp with the post. What your seeing is from the generic post that had a lot of issues. I'm not sure what version I'm running, newest from EMI, but I don't recall and I'm gone for a week. Post up you a bobcad example and your fusion version so I can see them side by side. Considering chapter 7 is dedicated to cutter comp... there may be a lot of possible differences.Quote:
Originally Posted by nlh
Nate, the option Make Sharp Corners on the passes tab is currently not doing anything in the post. I would expect this to toggle G48/G49. Do you know what the default is. My manual implies that rounding in the default (G49).
Quote:
G48 (Corner Rounding Off) edited into a program eliminates many of the problems with corner rounding in
controller cutter compensation and, being the default condition for BOSS 4-7 compatibility mode, adjacent moves
are made as they are defined. Reference: In controller operation, G49 (Corner Rounding On) is the default mode
and all adjacent non-tangent moves are connected automatically by an arc move in Cutter Compensation.
Nate, can you post a sample of cutter comp from bobcad? I have the Make Sharp Corners switch sorted in the post, I would like to verify the cutter comp operation. You mentioned the default cutter comp didn't look like you expected.Quote:
Originally Posted by forhire
Sorry forhire, somehow I missed your last couple of posts. I have been very busy of late. I have a bunch of programming to do today so I'll take the time and post up some sample code while I'm at the computer.
Thanks for all your hardwork!
Nate
Ok, below I have a copy of a sample program I just posted with Fusion 360. It is just a simple 2" x 2" x 1"tall cube. Profiled around the outside with a 1/2" endmill. Comp in this case is for "wear". Normally that's all I use it for. The lines in question are highlighted in red.
;(103)
;(Thursday, August 03, 2017 12:29:41 PM)
;(Fusion 360 CAM 2.0.3174)
;(Untitled)
;(cad)
;(T1 D=0.5 CR=0. - ZMIN=-1. - flat end mill)
G0 G17 G30 G40 G45 G72 G75 G80 G90 G96
G70
N1 ;(2D Contour1)
M9
T1 M6
S7640 M3
G54
M8
G17
G0 X-1.425 Y-0.05
Z0.2
G1 Z0.0394 F92.
Z-0.95
G18 G2 X-1.375 Z-1. I-1.375 K-0.95
G17
G1 G41 X-1.325 Y-0.075
G3 X-1.25 Y0. I-1.325 J0.
G1 Y1.
G2 X-1. Y1.25 I-1. J1.
G1 X1.
G2 X1.25 Y1. I1.
G1 Y-1.
G2 X1. Y-1.25 J-1.
G1 X-1.
G2 X-1.25 Y-1. I-1.
G1 Y0.
G3 X-1.325 Y0.075 I-1.325 J0.
G1 G40 X-1.375 Y0.05
G18 G3 X-1.425 Z-0.95 I-1.375
G0 Z0.2
G17
M9
M5
G90
M22
The way the code should read is below (highlighted in blue):
;(103)
;(Thursday, August 03, 2017 12:29:41 PM)
;(Fusion 360 CAM 2.0.3174)
;(Untitled)
;(cad)
;(T1 D=0.5 CR=0. - ZMIN=-1. - flat end mill)
G0 G17 G30 G40 G45 G72 G75 G80 G90 G96
G70
N1 ;(2D Contour1)
M9
T1 M6
S7640 M3
G54
M8
G17
G0 X-1.425 Y-0.05
Z0.2
G1 Z0.0394 F92.
Z-0.95
G18 G2 X-1.375 Z-1. I-1.375 K-0.95
G17
G41 X-1.425 Y-0.05
G1 X-1.325 Y-0.075
G3 X-1.25 Y0. I-1.325 J0.
G1 Y1.
G2 X-1. Y1.25 I-1. J1.
G1 X1.
G2 X1.25 Y1. I1.
G1 Y-1.
G2 X1. Y-1.25 J-1.
G1 X-1.
G2 X-1.25 Y-1. I-1.
G1 Y0.
G3 X-1.325 Y0.075 I-1.325 J0.
G1 X-1.375 Y0.05
G40
G18 G3 X-1.425 Z-0.95 I-1.375
G0 Z0.2
G17
M9
M5
G90
M22
In my experience the DX32 control wants the current XY location that the machine is at, on the same line as the G41 or G42. It also will want a G0 or G1 lead in segment on the line directly following the G41/G42, before you actually get to your part. This last item will not cause an alarm if it is not included, but you may very well end up with a scrapped part. I believe if the next line after calling cutter comp is an arc, the control will alarm out. Also a linear lead-out after exiting the part before calling G40.
When cancelling with a G40, it works best if it is done before any Z move. If you don't cancel before a Z retract, the machine will actually feed to the Z program location even if a G0 is called (i.e., G0 Z.1 will in effect become a G1 Z.1).
Another thing, you can't use cutter comp when performing a helical move. It's in the manual and also confirmed with Bart at EMI a few years ago. So if you plan on using cutter comp, the post either needs to be written so as to avoid this situation (call comp after helical ramp), or just be aware when your setting up a 2 axis contour to not select a helical ramp entry.
The manual does not do a very good job of defining items such as the G41/G42 line XY coords. At first attempt, I had terrible results trying to use comp. I tried running code just as I would on my Mazak. Really pulled my hair out. After many google searches and forum searches I managed to put the above together and it works. Would be great to hear from others to see if their experiences are the same. Typically I'm always pushed to get the jobs out, so when I find a combination that works and works consistently, I stick with it. Doesn't mean that there isn't another way :)
According to the manual, G49 is the default control setting.
Hope this all makes sense forhire!
Nate
I looked over the helical code. It is not disabling cutter comp as it should. This will take some work. And the rest of cutter comp definitely needs some work. One of the issues I have is with NCPlot that I use to back plot... it's not playing nice with the radius lead in/out for some reason, making it difficult to ensure the code is posting correctly. Does the code you posted back plot clean in bobcad? I'm getting a circle after the arc plane shift G18 to G17. This isn't the first time NCPlot has had issues... it doesn't support cutter comp so that may be the issue. Do you have a back plotter that work well with the DX-32 code? I've never had luck with the one on the machine.Quote:
Originally Posted by nlh
I have reworked the cutter comp. It's back plotting correctly. This has not been tested on the machine. I've include the fusion model for review. Be sure when you are using cutter comp that you toggle useHelicalMoves=no, otherwise it will post G12/G13 arcs on the XY plane when it shouldn't. ;)
The use sharp corners option toggles G48/G49 on the operation. When checked G48 in inserted, otherwise it calls out G49.
Let me know what needs adjusting. Enjoy.
UPDATE: I fixed the issue when using radial lead in/out. I added a linear move to the current position on the plane shift G17. Previously I had the linear move on the next block but it would make a circle. Change is bolded. I uploaded a new zip file containing the change this morning.
G19 G3 Y-1.775 Z-1. J-1.775 K-0.875
G17 G1 X0.25 Y-1.775
G49
G41 X0.25 Y-1.775
G1 X0.275 Y-1.525
Does anyone use G9 to make the movements smother. If I don't turn it on finished passes get small facets because of the acceleration and deceleration.
Sent from my SAMSUNG-SM-N900A using Tapatalk
I haven't messed with it. What type of finishing operations have you required adding it? Are you enabling it for the entire operation or just troublesome spots? Ideally if one could identify the trouble spots it could be disabled using G99 for those movements. Are you seeing it on arcs or short segments?Quote:
Originally Posted by cooperjm
G8 Deceleration Override OFF (default)
G9 Deceleration Override ON
G99 Deceleration Override, Single Block
It would be interesting to develop a test model so some cuts could be done and compared. I'm certainly interested in improving surface finish. ;)
I just checked the post source and it is not being used at present.
Currently I'm using another program to post code. I want to start using Fusion 360 exclusively though. I have been using G9 on roughing pass and finishing passes. It's moved out the jerkiness of the machine to me.
I have not posted anything with fusion and ran in the machine. I will try a simple Contour with your post and see what results I get. Maybe I can upload a video to show the deceleration issues I'm having. The faster the feed rate is the worse it appears. The G9 could be covering up some other issue.
Sent from my SAMSUNG-SM-N900A using Tapatalk
Here is the post output that I just used to cut a 3" diameter pocket. It works but there is a slight hesitation between every feed line.
G9 has to be turned off before any rapid move.
:1242
N10G17G80G90
G0T04M06
G8
G54
S4500M03
G90X.685Y.6453
Z.1M08 I usualy insert G9 in this line
G1Z-.25F5.0
G41X.685Y.6453
X.6906Y.6535
G3X.7258Y.7667I.5258J.7667
X.6389Y.9316I.5258J.7667
X-.0006Y1.13I-.0006J0.F15.0
X-1.1306Y0.I-.0006J0.
X-.0006Y-1.13I-.0006J0.
X1.1294Y0.I-.0006J0.
X.6389Y.9316I-.0006J0.
X.5541Y.9845I-.0006J0.
X.4559Y1.0102I.4559J.8102
X.2817Y.9084I.4559J.8102
G40G1X.2768Y.8997 I usualy insert G8 in this line
G0Z.1
M09
M5
M22
G90G0
M30
The videos below show the effect of G9. I have been using G9 even in roughing, it cuts down the cycle time.
This path comes from Volumill
Attachment 369728
This is 2D Adaptive from Fusion
Attachment 369730
Adaptive with out G9
https://youtu.be/eqS5R4idkG8
Adaptive with G9
https://youtu.be/4m45acnWqSk
This is part of the code running in the video.
:1242
N10G17G80G90
G0T04M06
G8
G54
S2000M03
G90X-.3375Y0.
Z.1M08
G1Z.1F75.0 Insert G9 here
Z.01F100.0
G3X0.Y-.3375Z.005I0.J0.F17.8
X.3375Y0.Z0.I0.J0.
X0.Y.3375Z-.005I0.J0.F35.5
X-.3375Y0.Z-.01I0.J0.
X0.Y-.3375I0.J0.F17.8
X.3375Y0.I0.J0.
X0.Y.3375I0.J0.F35.5
X-.3375Y0.I0.J0.
X-.1687Y-.1687Z0.I-.1687J0.F100.0
G1X.225Y-.1125F200.0
G3X.3375Y0.Z-.01I.225J0.F50.0
G1Y.089
G3X.2234Y.342I0.J.089F23.7
X0.Y.4265I0.J.089F47.4
X-.3375Y.089I0.J.089
G1Y0.F100.0
G3X-.225Y-.1125Z-.0011I-.225J0.
X-.2032Y-.1104Z0.I-.225J0.
G1X.2468Y-.0213F200.0
G3X.3375Y.089Z-.01I.225J.089F100.0
Very interesting. Now I'm going to have to run some code with and without. It certainly makes sense. I assume your running from memory and not using DNC?Quote:
Originally Posted by cooperjm
One thing I found interesting was your post from Volumill. The helical arcs are using G2/G3. The helical arcs in the fusion post are using G12/G13. I've always used G12/G13 when thread milling using polar angular motion in number of degrees. It's handy because you can thread mill in two lines of code. With CAM calculating the path it's not really required. I prefer the G2/G3 method because it back plots perfectly. My post for Visualmill handled helical for thread milling but did segments for the helical lead ins. It would be nice to have this sorted. I'm going to try the G2/G3 arcs in my post and see how it goes. Any thoughts?
Quote:
G0(G1)R__I__J__A__Z__ (F__) ;Move to Helix Start Point
G12(G13)A__Z__F__ ;Do Helix
G1 is the G-Code for XYZ Linear Interpolation (Feed);
G12 is the G-Code for Helical Interpolation in a Clockwise Direction (CW);
G13 is the G-Code for Helical Interpolation in a CounterClockwise Direction (CCW);
A__ is Polar Angular Motion defined in terms of the total number of degrees of
helical travel (for G12 & G13 only). This is an “unsigned” incremental value;
Z__ is the absolute depth of travel;
F__ is the Feedrate;
R__ is the Arc Radius; and
I__, J__ are the X & Y distances (respectively).
I loaded the program from A:, it was not DNC.
Sent from my SAMSUNG-SM-N900A using Tapatalk
Floppy? What's that? Ha Ha. Best thing I did was to network my machine. Life is too short for floppies. ;)Quote:
Originally Posted by cooperjm
I spent some time tonight testing the G9 deceleration override. I wasn't able to duplicate the issue on my TC-3. Can you post the full code from your test video and I'll try again. I ran with and without and my adaptive path finished at exactly the same time and the movement was fluid, I'd like to say it made difference but if it did it didn't show up in the clock.
I converted the helical code to use G2/G3 arcs. Worked perfectly. I even use a helical lead in. Much better than the polar angle method using G12/G13 which require a straight in lead. Bonus is that it back plots perfectly. The interesting thing was the code was never actually using a mode that required G12/G13, all I did was change the call out to use G2/G3, no other changes.
I spent the most time de-bugging the cutter compensation. Boy is it picky. The errors are cryptic. After a couple hours I finally have it sorted. In the end it was the order of things. Tested on my machine with a 2D contour. I'll likely try a few more tests next week.
I've attached the latest post code.
UPDATE: I have moved my post files to my web space for easier versioning. For the latest version you can check here:
http://home.lewiscounty.com/~forhire/posts/
Direct download here: http://home.lewiscounty.com/~forhire...eport_dx32.cps md5sum: 43fa8157dfacb1a17d11763f04302367
Attachment 369744.
No floppy, usb emulator. I would like to network it. I have read your post on what you did to your machine. I just haven't sat down to figure out how to network this motherboard.
Also I don't think your latest post attached.
I was likely editing the post when you looked. I've moved my posts to my web space.Quote:
Originally Posted by cooperjm
http://home.lewiscounty.com/~forhire/posts/
cooperjm, I added the G8/G9 feature to my latest post. Set decelerationOverride=true and it will insert G9 on feed speed moves and g8 ahead of rapid moves. It is modal so it will only appear when required. Please test and let me know. You can download from my posts folder. http://home.lewiscounty.com/~forhire/posts/
I will give it a test as soon as I can. I will let you know what I find. Also I will give the cutter comp a test. Thanks for you work on this post. This has been one thing that has kept me from using 360 for CAM.