Ahh here is the post where this was first mentioned: viewtopic.php?f=100&t=3488 We will have to change the downloaded version if we did not already. I checked my local copy and it was still the old way. (fixed now thanks nf119!) Mark and Trish
I had totally forgotten about this. I didn't follow it up after I've posted in that thread and didn't make the changes. I'm such a tool, somtimes. BTW, Mark. I had mentioned it before. I made some changes to the script so that it will not retract when multipassing after each pass. After I posted the change Shaun had said that when it drills holes it should retract and I had made the change so that holes retract, pick drilling, but the cutting does not retract. I never posted the corrected change since no one downloaded the original anyway. If you want, I can post the changes and they can be included in the upgrade too. Doesn't have too, if there is no interest. I've been using it for over a year now, with no problem. I sometimes cut 3/4" wood with more than 20 passes and it make a difference to me when the bit doesn't retract between each pass. It make no difference if you cut without the multipass.
I too had forgotten about this Yoram. So its not just you my friend we are all getting older I guess (well that's what I blame it on anyway) That would be great! I will update it in the SketchUcam section once you post! Thanks Brother Mark and Trish
Thanks! I've just started to use SketchUCam, but haven't been able to generate a single file before that didn't have the kind of errors you got. Now I'm gonna try out my mill!
Hey, what do you mean 'we are all getting older'! Speak for yourself! I'm getting younger and I have solid proof for it. They used to say to me 'Yoram, you are such a man!' and now they say 'Yoram, you are such a baby!'. Ladies and gentlemen of the Jury, I rest my case! :tease: The code change I made to prevent the retract to safe hight during multipass milling. [pre] # If it's peck drilling we want it to retract after each plung to clear the tool if (phlatcut.kind_of? PlungeCut) aMill.retract() aMill.move(point.x, point.y) aMill.plung(cut_depth) else # If it's not a peck drillling we don'lt need aMill.move(point.x, point.y) aMill.plung(cut_depth) end else The above code has to be inserted between this code... [pre] # transform the point if a transformation is provided point = (trans ? (cp.transform(trans)) : cp) # retract if this cut does not start where the last one ended if ((save_point.nil?) || (save_point.x != point.x) || (save_point.y != point.y) || (save_point.z != cut_depth)) if (!cut_started) if PhlatScript.useMultipass? [/pre] and this code if the GcodeUtil.rb aMill.retract() aMill.move(point.x, point.y) aMill.plung(cut_depth) end [/pre] You can also download the .rb file and replace it with the one you already have. It's located, typically, in Crogram Files (x86)GoogleGoogle SketchUp 7ToolsPhlatboyztools Attached files GcodeUtil.rb (11.5 KB)Â
Please note that this version viewtopic.php?f=98&t=2297&start=50#p43518 of Phlatmill.rb fixes this bug too (-: EDIT: that link is now broken by the forum upgrade. However, you can still get the fix
tyring to work out what is going on hardware FleaBay CNC6040 + G-540 + all cables replaces with high quality shielded cables software Google SketchUp 7 + PhlatscripT + Mach3 2 files 1 is the raw gcode and 1 is the modified code by hand !-table-leveling.cnc is the raw file output but when i run it about 2mm before each corner it misses or jumps a step !-table-leveling-MOD.cnc is the same file hand edited to remove all of the up and downs of the Z axis that where not needed and to remove all of the (Pass 1) out of it nothing else is changed the raw file i have to run a feed rate of 100 mm per min or less (if i go over 1000 mm per min the cnc makes LOTS of horrible noises) the MOD file i can easly run it at 2500 mm per min and it runs no trouble at all the 3rd file is the SketchUp 7 drawing file if you want to see what its made the gcode from my question / bug is why is it doing the missed steps in the raw file PS:- if you need i can post a vid of the 2 files running so you can see and hear what happens
seems to me you're having resonance in your motors, particularly Z. some things I noticed in your file: plunge rate is set to 2540mm/min - can your Z axis do that speed? the feed rate is set at 1000mm/min, might be a bit fast if G64 is in effect. you have set multipass on, yet your centerline cuts appear to be set for just 10%. 10% of 1mm material thickness is 0.1mm, the same as your multipass depth. Having multipass ON will make for lots of Z motion as it lifts and plunges at the end and beginning of every line segment (a bug not yet fixed) but it is only doing one pass of 0.1mm anyway. I recommend you turn multipass off. You do not have G61 defined so Mach may be trying to maintain speed in the corners by 'cutting the corner' (G64 mode). In your Constants.rb file, set 'Use_exact_path = true' to force Mach to go to and stop at every end point. making noises at high speeds near corners may indicate your acceleration rates are too high. Looks like you hand drew that whole thing! wow, but there are alternate ways to do it. One would be to use the 'pockettool' to draw zigzags over the surface. pockettool if you don't want zigzags you can still use the pockettool, just hold down CTRL to only draw the boundary, multiple times. Another way is to use a specific flattening tool, like this one which is written in Python so you will need to install Python first. While I have run the tool, I have not run the code it generates on anything so check and test before committing to a real cut. However, I have made changes to the setup and generated the Gcode for you and you can get it from mywebserver (I still cannot upload any files, though it seems others can, Mark). Note that I am using Phlatscript plus the latest bug fixes and extentions, called 'TRUEPLUNGE'. I don't think this has affected the way this code is generated, but you may want to install this and see if it benefits other stuff you do. Just search the forums for 'TRUEPLUNGE'. Please let me know if this code works correctly.
nope z isnt even moveing when it happens its at a few mm before the end of each run and the noise comes from the axis that is moving X or Y 1: Z is limited to 500mm p.m in mach3 2: G64 isnt in the gcode unmodified makes the noise running at more than 200mm p/m (Pass: 1) X1.500 Y1.500 Z10.000 G1 Z-0.100 F2540 X548.500 Z-0.100 F1000 G0 Z10.000 (Pass: 1) G1 Z-0.100 F2540 Y378.500 Z-0.100 F1000 G0 Z10.000 (Pass: 1) G1 Z-0.100 F2540 X1.500 Y378.500 Z-0.100 F1000 G0 Z10.000 (Pass: 1) G1 Z-0.100 F2540 Y2.000 Z-0.100 F1000 G0 Z10.000 after striping out the code in red i can run it at more than 2500mm p/m X1.500 Y1.500 Z10.000 G1 Z-0.100 F2540 X548.500 Z-0.100 F2500 Y378.500 Z-0.100 F2500 X1.500 Y378.500 Z-0.100 F2500 Y2.000 Z-0.100 F2500 3: yep i could have turned off multypass but it shouldn't be causing this trouble because its happening before the Z dose anything i'll post a vid of it making the noise if you want 4: running my edited code i can do it at 2500.. or more with no trouble at all and it dose not cut corners 5: no i have spent a lot of time finding out at what acceleration rate i can run at max then took 20% off it LOL yep that is 1 word for it took me hours to make it but i have it now and wont have to remake it again tryed it but it for some reason even tho my bit is set at 3mm it is doping the out side edge at 1.6mm not the 1.5 it should be so i just made what would work lol [/quote]However, I have made changes to the setup and generated the Gcode for you and you can get it from mywebserver (I still cannot upload any files, though it seems others can, Mark). Note that I am using Phlatscript plus the latest bug fixes and extentions, called 'TRUEPLUNGE'. I don't think this has affected the way this code is generated, but you may want to install this and see if it benefits other stuff you do. Just search the forums for 'TRUEPLUNGE'. Please let me know if this code works correctly.[/quote] ok i'll have a look at the bug fixes got the gcode and made it in to a file but its to late at night to start the mill (people next door would skinn me) will try it tomoro thanks for looking
aha! then it is the step rate on x or y that is resonating. steppers have a minimum step rate below which they get very noisy and can miss steps. similarly they have a maximum rate, and of course depending on the load on them, a maximum acceleration. I'd halve the acceleration on X and Y and see what happens. then up the minimum step rate and see. etc. change only one thing at a time (-: it doesn't have to be since it is modal, once it is set Mach will remember it forever, you have to set G61 to clear it, then it remembers G61 forever that will be interesting! there is a version of Mach that does not limit feeds correctly when all axis are moving together, but that was an older one and I assume you have a newer or latest version. This was particularly in reference to a slow Z and there is special code in the Phlatscript Gcode generator to handle this Mach version for Vtabs. since the pockettool is NOT PART of Phlatscript it does not use the phlatscripts settings for bit size, you have to edit the pockettool.rb file to set the bit size. However, I have started integrating it into PHlatscript so this will work at some point in the future. LOL. dang neighbors, always fussy.
hmm i went to rerun the file that was giveing me all the problems but its not doing it any more must have been something in your file that fixed it so thanks love the TRUEPLUNGE
i am a EX motor mech yep i HATE INTERMITTANT faults , squeks , thumps , ect.... i can run the mill up to 3500mm no prob 3600mm the hole unit resonates 3700mm and up it all go's smooth again now all i need to do is find someone to teach mt how to cut Ali and not brake bit's
not too difficult, I often cut Al with my woodworking router and carbide bits. The trick is in preventing the ali from sticking to the bit. On my lathe I use kerosene as a cutting fluid for Al, but the router would throw it everywhere so I just rub the surface to be cut with beewax or a candle (before each cut since it leaves the area on the chips) For CNC, it is better to calculate the feed rate instead of guessing. Feed rate depends on - number of teeth - RPM - material - depth of cut per tooth. There are several calculators on the web, just google. And remember there is such a thing as cutting too slowly! The other item is to climb cut if your machine can handle it. This makes the chip 'thick to thin' instead of 'thin to thick' and among other factors, clears the chips much better. If you can use a bit designed for ali so much the better. Have fun (ps I'd love to see a pic of your machine)
umm ok i dont know if its something i did wrong but umm . . . well look at my files scroll down the CNC file you will see what i am talking about (all the (Pass x) not where they should be) i have had had this randomly in some of the last 6 files i have made in the last few days
yup I know about this. I have implemented the new feature of being able to set the depth of plunge holes, and/or the size. so you can drill a 50% depth hole that is 8mm diameter, with a 3mm bit. However, the way multipass WAS implemented it did the plunge holes along with all other 'per pass' stuff, but now all plunge holes are handled by the 'plungebore' routine which doesn't know about putting (pass x) in the right place, especially in this rather unique file in that there are no other cuts. basically the plungebore routine does all passes for a multipass hole in one go, and then lets the regular plotter do the other mulipasses, so the plunge hole is all done in 'pass 1'. Unless this is causing actual problems in your CNC interpreter I'm not going to worry about it until my long list of new stuff is working nicely. it is just cosmetic, really.
ok cool just didnt know if it was my mistake of adding it or what thanks for letting me know its all cool and will come out in the wash latter lol PS:- thanks for your hard work
When I call up the Phlatbone Tool, there is always the number 3.18503937007874 in the window, regardless of any prior changes that I have made. When I change this to the tool diameter, the Bone operations work as expected for that tool diameter, but when I call the the Phlatbone Tool again, the magic number 3.18503937007874 is back. Any clues?
3.18.....is 1/8" in millimeters. If your bit is set to 1/8" in the parameter box than it's correct what you see.
Ah, I see that now. However, the impact is that it sets the Bone diameter to 3.18... inches, unless I reenter 0.125 each time .
Kenn, why do you want to force it into inches? Do you really care if it is made in millimeters or inches, as long it's the right size? Even if everything else is in inches, it still picks up the bit diameter that you have in the SketchUcam parameter and converts it to millimeter and draws it in the right size.
I don't really want to force it into inches. I was just pointing out a minor, but potentially troublesome bug. A bit of further testing, where I set the Tool Diameter to 0.25 inches, and the dialog box came back with the 3.18... in the window. Now that I know the work-around, I know that it won't cause me problems. It may still affect others.