Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Briancnc on November 10, 2008, 08:54:12 PM
-
Well this originated from a vectric forum thread but it seems the problem isn't in the vcarvepro file its in the post processor or the gcode/settings I have in mach3. It's two part, one that the pockets aren't complete and they are cut weird and all the same way. Second there are knicks or bumps at the end of each corner, like it took almost 1/16" about 1" long off the edge of each of the parts.
I stopped the program after the two parts cutout on the bottom so I could rectify the pockets without rerunning the entire program. Anyone have any idea what's going on? I attached screens pics and the tap gcode file. Thanks!
http://vi01.com/cnc/mach/4thaxispartsUPDATED.tap gcode file (gcode ATC post processor from vcarvepro)
(http://vi01.com/cnc/mach/DSC_0995.JPG)
(http://vi01.com/cnc/mach/DSC_0996.JPG)
(http://vi01.com/cnc/mach/DSC_0997.JPG)
(http://vi01.com/cnc/mach/DSC_0999.JPG)
(http://vi01.com/cnc/mach/machscreen1.JPG)
(http://vi01.com/cnc/mach/machscreen2.JPG)
-
Briancnc,
Does your CAD file look like this?
Note the small straight line segments for the curves.
RICH
-
My cad file doesn't look like that, that's a gcode generated by VcarvePro out of a gcode post in that program. Even if there are those little line segments that doesn't explain the little pocketing anomaly nor the little nips towards the corners. But appreciate you looking at the gcode.
-
Briancnc,
Early and need to get to work, but, i wanted to see if there was something in the code which did the offset your getting. Have some other thought's but need to get going.
RICH
-
Thanks Rich.
Recut tonight with mach3 arcs atc gcode post as usual (this is the PP I have been using since I have been using vcarve and mach3, probably more than 2 years now) and it ran the same. Also note in the pics its just a random pocket path, also check out those stepdown marks and how it cut those sharp corners and made them round even though vcarve prview shows them sharp.
Really strange, never seen this before on my machine.
(http://vi01.com/cnc/mach/badparts1.JPG)
(http://vi01.com/cnc/mach/badparts2.JPG)
(http://vi01.com/cnc/mach/badparts3.JPG)
-
Turn off all the CV options, both on the settings page and in the general config page. But leave CV on. If it's still the same, turn CV off and try it.
-
Braincnc,
You may want to take a look in documentation "Mach 3 CV notes".
Also just try something with equivilant cuts using Exact Stop and compare the cutting. It will be jerky going around the corners because of all the straight lines you have instead a smooth arc. Particle board ( particularly cabinet grade) has some darn hard stuff in it, such that it seemed it's possible to push back should there be any play or backlash. Additionaly, if the router assembly isn't solid you can get some spring back when say if the axis is slowing down and the cutter has more time in an area. Also saw what looked like a soft spot in the one corner and that could even contribute more to it. Have you played around with lesser depth of cuts? ie; get the accuracy you want first and then best speed will come.
Rather than making dust, use a pencil in the non working router / no z moves to trace around see how the profiles are under no cutting pressure. First step would be elimination of any Mach settings as already posted and then some playing around on your part to see what works.
Just some suggestions,
RICH
-
Gerry and Rich thanks for your replies. I will look into the CV settings tomorrow hopefully I can narrow it down. I just haven't had a problem with this setup in mach3 before; that's what got me. Maybe I inadvertently turned something on? will have to check. Thanks so much.
-
Ger I have nothing on the settings page on for cv if any at all, neither in the gen config either but it is green lit in the CV mode (not dwell). Rich I'm not sure its necessary to test with a pencil, I know the feeds and speeds this machine can do; I mean I have cut quite a bit with this machine before with no problems. And frankly I haven't changed any of the settings. It's just strange because one; it shows in my vcarve preview that it's perfect, it shows in my mach preview that it is cutting normal yet it doesn't. There's just no consistency to it really; it will cut fine in certain areas and weird in the same type of area elsewhere. Sometimes I think these machines take a mind of their own.
-
Well I just investigated further. Check out how it deviates from the programmed toolpath. Wow, what could cause that? Never seen mach color outside the lines! lol
(http://vi01.com/cnc/mach/toolpathscreen.JPG)
-
(http://vi01.com/cnc/mach/toolpathscreen2.JPG)
(http://vi01.com/cnc/mach/toolpathscreen3.JPG)
Some more, well that explains it. Now i know its not my machine..
-
anyone :D?
-
If you make changes to CV settings make sure you close Mach and reopen it. As it seems to have problems saving these settings mid session.
If mach is not staying tight to the tool path you either need to slow down or turn on CV dist tol. The value for this is part dependent. I would guess for your part size about 0.10" would be a good place to start. Again if you make any CV settings changes close and reopen mach.
-
Hmm.....depending on the corner radius, look ahead, and what needs to happen to keep velocity the path may be
automatiicaly changed.....not sure what i said is correct
rich
-
Not read through the rest of the post so if its already been said please forgive :) Ok for a test have a look in the code and see if there are any G64's if there are replace them with G61, also make sure there is a G61 before the first cut. If that cures your rounding then it shows that its a CV problem due to the acell of your particular machine and you will need to try and tune the CV settings to suit.
Hood
-
Sorry for the delay in followup. I appreciate your help. Anyhow I ran it again using suggested settings of cvangle to 35 and dist tolerance of .01 but still having issues. As you will see below the parts cut perfectly but it was choppy, feeds from 200IPM down to 25IPM at curves it didn't handle it how I would expect other than that it followed the toolpath perfectly.
I guess what I'm getting at is that I'm having a hard time finding a balance between acceptable constant velocity and necessary cv. I want it to go fast because the machine is designed to do so but the software skips the beat because the machine can't make those corners without either slowing down or cutting them. And the strange part of all of this is until now I have never had to play with CV settings, everything I have ever cut has been perfect; mach seems to always have compensated for corners and curves slowing down when necessary. Where am I going wrong with this? Thanks again!
(http://vi01.com/cnc/mach/DSC_0004.JPG)
-
Understand you want to go fast, but I'm a slow poker who prefers accuracy, repeatability and reliability over speed.
So find a speed that gives you that then fool with the settings until cutting is achieved. Now bump the speed gradually
up until you find the max speed for what you are cutting and back off say 20% for that particular material. What you are cutting may require a slower speed. Again, if you were cutting using circular interpolation ( G2 / G3 ) instead of cutting small straight line segments it would not be jerky. Your motors would be singing to you.
RICH
-
I don't know if this has any relation to your problem, but I've been evaluating Mach3 and I had exactly the same result you got; namely what appeared to be random deviations from the desired path . .
It did not occure in any programs that I wrote but did appear in any wizard programmed code.
Eventually I noticed that there was a pattern to it. The tool was turning WAY early like you do in your car if you were driving REALLY fast, and that led me to check into the feed rate, motor speed and accelleration settings.
I use feed per rev and the wizard put out IPM, so the wizard stuck the feed at say 50 in the code which is 50inches PER REVOLUTION in feed per rev. That's what was causing the tool to go off path in my case. I would not swear to it, but I don't think I got any errors . . . it just ran fine, but with the tool doing exactly what yours is doing.
In messing around trying to figure the problem out, I notuced that (if I am remebering right) that the accelleration set in the motor tuning also can cause the tool to meander is Mach thinks the motors need more time to accell decell than they really do.
So you might check your motor tuning settings and see if something has changed there.
-
try this setting