Machsupport Forum
Third party software and hardware support forums. => Newfangled Solutions Mach3 Wizards => Topic started by: BobsShop on February 17, 2007, 10:15:31 AM
-
Having a problem with the Cut Circle Wizard in the Suite of Handy Wizards: I have copies of Mach 3 V 2.0.047 on two different style computers and have the problem is constant. I have tried running in simulation mode (without mill attached) and in real time (with mill running), changed CV numbers, changed from Constant Velocity to Exact Stop, Absolute to Incremental. The work piece was been moved away from the xy limits to insure not running out of room.
This code was produced by the wizard - no edits have been made. The depth of cut was reduced to save time while running and watching. If doing a simulation the arc traverses half of the circle then crashes and freezes. This also happens when running in real time.
I have tried other circles in the Wizards pack (German Bravo's, etc) and they produce workable code. I just prefer the simplicity of Brian's original work.
(Program Posted for Aluminum )
G0 G49 G40.1 G17
G80 G50 G90 G98
G20 (Inch)
(***** Circular Groove/Cutout *****)
M6 T12
M03 S3000
M8 (Flood On)
G00G43 H12 Z0.3
G00 X0.2844 Y-0.1078
G41 P0.09375
G01 X0.3922 F16.9
G01 Z-0.002 F8.45
G03 X0.5 Y0 R0.1078 F16.9
G03 X-0.5 Y0 R0.5
X0.5 Y0 R0.5 ( IT IS AT THIS POINT THAT THE PROBLEM OCCURS. )
G03 X0.3922 Y0.1078 R0.1078
G40
G00 Z0.3
M5 M9
M30
Any and all suggestions will be appreciated and explored.
Thanks
Bob@ BobsShop - cutting circles and losing my mind.
-
I didn't look at it close, but there is no g (GO) command on the line you have marked as the troubled line.
Brett
-
I think that line is actually a G03, and its OK to leave it off because G03 is modal. I tried the code and it hangs for me too. I added the G03 and the problem still occurs. I think this one should be shown to Art, its not a wizard problem, the Gcode looks good. There was a recent problem like this that Art fixed.
I put a note on the Yahoo group for Art.
-
Thanks Ronginge - that was what I was going to say (no additional code needed for modal entries). Deleting the Part Offset entry (G41 PO .1875) enables the code to complete the arc. But, of course, that defeats the purpose of the code since there is no compensation. I even went into the General Config. and checked and unchecked the "Remove Tool Offset" entry, It did not appear to have any effect.
Thanks again for looking into this and confirming I am not losing what little sanity I have left.
Bob@BobsShop - Sitting back and waiting for Arts solution.
-
Ok, Art just posted this on the Yahoo group_
Hi Ron:
I gave this a top priority, Id like to get the G41 as tough as I can. Version .048 fixes this problem. It turned out to be the same square root error as before, only in a slightly different way. I have tightened it up a lot, so this can't or shouldn't happen again . Thanks for the bug, download .048 and that arc will work fine..
Art.
-
Beautiful circles again.
Thanks Ronginger and Art:
I had continued to play with this wizard just to see how convoluted I could get it and was going to post some additional information in order to guide the debugging. Should have known that Art would not require any assistance. Having written software for financial applications in another life, i know how frustrating and labor intensive finding a bug can be. I really appreciate the dedication and effort demonstrated by everyone involved with ArtSoft and Mach 3.
Bob@BobsShop. It may only be a hobby, but it is my hobby.
-
I'm having a problem with cut circle. When set up the wizard and then push "preview" the picture looks correct. Lead in and offset good. See the first picture below, named "correct.jpg". Then I push "back" and post the code. This brings up the NFW page that has all the wizards on it and the "verify toolpath" button. When I click the "verify toolpath button" the toolpath initially shows like the first picture below it very shortly changes to the second picture below, named "incorrect.jpg". When I exit to mach it looks like the second picture. I have tried changing arc between absolute and incremental but there is no change.
So what setting do I need to change to fix my little problem.
-
Gim, I have had similar (but not exactly the same) things happen when I have partially ran code and stopped before an M30 code was read. Seems that running code without the terminating M30 being activated leaves commands that may interfere with a new program. Not sure if that is what is happening to you, but it is something you may want to consider.
Seems I remember reading recently that version 3.0 had produced some problems - I don't recall the particulars of that post. Version 3.0 was removed from the download choice and replaced by 2.63. That said, I am still using 3.0 and have not experienced any problems - YET!!
What are the particulars that you are inputting into the Wizard?
Bob @ BobsShop - Still making chips and cutting circles.
-
Thanks for the reply.
I don't think M30 is a factor as it happens even when I use cut circle first thing after a reboot.
Settings are:
cutter diameter 0.25
center of circle x0y0
diameter 1.125
conventional milling
cut inside
top of part 0.000
safe height .020
depth .05
step .05
pitch 0
Thanks,
Spence
-
Just a stab here, do you define the lead in arc? If so, is it bigger than tool diam.?
Brett
-
Thanks for the idea. I don't see anywhere to specify the size or anything else about the leading anywhere in the cut circle wizard.
Spence
-
This one is driving me nuts. I took out all the G41/2 cutter comp moves form the threading wizard to eliminate these kind of problems. I do not yet understand what is happening, but it has to do with the cutter comp. I have been discussing it with Brian and I know he is planning to look closer at the comp code, but I dont know when he will get it done.
The leadin radius is set by the wizard to be 115% of the tool dia, so it ought to work for any tool size.
A recent thread on the yahoo group has been talking about the inc or abs mode issues, I need to go through the wizards and be sure they are consistently using that. A while back Art changed the default initial Gcode string and that broke several wizards.
Sorry I dont have a better answer on this one, but we will get it eventually.
-
Thanks Ron,
I know it'll get sorted. I wouldn't have reported it if I was sure you already knew about it. Is there a list of known bugs I can refer to in the future so I don't end up taking time and bandwidth repeating old reports?
Spence
-
Hi, Gimble88.
Interesting - I used your inputs and got the same results. Did some additional tinkering (never could leave anything alone!) Editing the G-code and eliminating the reference to G41 altogether cleaned up the final result. Of course, this also did away with the lead in and you may want that. I then changed the PO to .0625 (1/2 of .125 - the size of your cutter). By changing the position-offset (PO) to .0625 you get a nice leadin and no garbage. This will not correct the view you get in the "Verify Tool Path," screen, but it should produce workable code for the finished product.
The Wizard appears to have a bug in it and Ron and/or ART will need to address that.
Bob@BobsShop - Going in circles - again.
-
I FOUND It !!!!!
The preview button code used a factor of 1.5 times the tool radius to calculate the comp radius. The post code uses 1.15 Apparently thats not a large enough move to make comp work correctly.
Ill send this fixed version to Brian to put on the web, but in the mean time there is a work around. The Preview button generates its code as Test.tap in the gcode folder. The post code generates its code into NewProgram.tap. If you preview the code, then post and return to mach, then load the Test.tap file you will get the right code for the comp move. However, that file will not have the coolant and spindle commands in it, since they are not necessary for the preview function.
I need to chack out some reported bugs in the thread code, lLl try to do that later tonight or tomorrow, then Ill post a new version in a new topic here with this fix and the thread fix. It should be up by some time tomorrow.
-
Hey Ron,
Brilliant work. Thanks for the rrrrrrrrapid response.
Spence
-
Hello all,
When Cut Circle generates G code it does an R instead of I and J,is there a way to change this to I and J?The problem is there is a hesitation at the half way points of the circle.I think Brian was told but am not sure.
Thanks
Troy
-
Dont know if this matters,but iam altering the Free 2D Milling Wizard by Olivier and noticed that it will generate a arc using either I and J or R,by using whatever you have the settings in the General Confige,Motion Mode,Distance Mode,and IJ Mode.
Can this be made the same for the Cut Circle NFS wizard?
Troy
-
It could be changed, but I don't see much reason to do it. Either R or IJ are valid gcode commands, both should do the same thing. If the R method causes a hesitation then we ought to get Brian to see why that happens.
-
Did this problem ever get resolved? I'm still getting the problem after downloading the 3.041 version today.
I'm trying to do a cut circle with center at x1.25, y1.25, diam 1.784, cutter diam 0.5, inside specified, climb cut specified, pitch angle 5 (although still have problem if this is set to zero).
I get a lead-in arc on the inside but then it keeps going and cuts another one on the outside.
Not so good, I ruined a nice piece of aluminum.
I've stated this before and I still strongly feel this way, you need to create a thorough test suite for these wizards and test them carefully before bundling them with Mach. Wizards are something you you need to be able to count on as being bulllet proof, but for me they've been my biggest source of crashes and ruined workpieces.
Paul T.
-
Did not have any problem when ran the Wizard. Nice circle, lead-in and lead-outs.
On a whim, I went back and ran the wizard again. Found if I specified an inside cut and posted the code (but did not exit to Mach3) then realized I meant to do an outside cut (or vice-versa) and went back to the circle and changed to inside then posted and exited to Mach3 the previous code was overlaid by the new cut.
Actually, I think this feature was built into the Wizard to enable code from one operation (say drilling a small circular hole pattern in a larger circular cut-out) to be added to code from a previous wizard. But, I am not the designer of any of the Wizards so my explanation may not make any sense of be correct.
Maybe Ron Ginger or someone else can better answer your question. You may want to post the errant code here so they can determine the problem
Bob@ BobsShop. The more I play with Mach3 and LCAM the "betterer," I like it!
-
Indeed, it is an important feature of the NFS wizards that you can run several of them in sequence and build a complex program. If you did not want one of the parts there is a way to list all the parts and to delete anyone of them. There are buttons to list and edit near the bottom of the main menu screen.