Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: Mauri on December 26, 2016, 09:12:57 PM
-
Hi,
Has something changed with CV G64 and Full Stop G61 on the Mach4 program?
Using Road Runner example.
Earlier versions of Mach4 you could run Exact Stop G61 and it would follow the line precisely in Simulation Mode.
Now on the latest versions of Mach4 it goes faster around on the lines (using the same Road Runner example) but does not track them?
It is like it is in some sort of CV Mode even though it is G61?
When trying out the CV Mode G64 I cannot get it to track the lines?
Has anyone tested what Speed settings on the Degrees in the CV Wizards would be required to track the Road Runner lines precisely or close?
When preforming 2.5D/3D engraving/carvings there are many thousands of varying cutting angles, similar to Road Runner so there must be some sort of settings that would do the task.
Can anyone help?
Regards,
Mauri.
-
Hi Mauri,
I can't help you but that are good questions. I played around with the CV-Wizard with the Simulator and I can't figure out the mystery behind it. How do I have to use the settings for the angles? There must be something wrong in my thoughts. In one test all angles were set to the same number - 500 and I expected this would be the maximum feed rate but the feed rate went up to the max velocity set in Mach-Config. But now the tracking is perfect as far as I can see on the monitor. I have no idea what's going on. ???
Can anyone explain the usage of the the CV-Wizard?
regards from Germany
Klaus
-
Hi,
I performed some more tests using a G-Code file that I made up.
This file performs much better than the Road Runner example?
I used Mach4 V3233.
G64 CV with 0 Degrees at 100 performed better than G61 Exact Stop, you have to enlarge each angled corner to see the differences.
Although the Exact Stop should be true to the G-Code profile in this case it does not.
Both performed better than Mach3.
Test File below.
I will have to see how it performs with 2.5D profiles and will comment further after I have made some tests.
Regards,
Mauri.
-
Mauri Try a Vcarve, M3 struggles with V carving, It was better in the M4 2.0 versions than what M3 could do at the same feed, velocity and file I have not tried the new version.
-
Dude1,
I have performed many 2.5D and 3D 4 Axis Carvings using Aspire and madCAM with Mach3 and have been able for Carve in Brass and Timber for many years with reasonable results.
On the Brass we finish the output using a stereo microscope and fine needles as well a special stones that you can make into a fine point.
On Timber we use fine paper to improve the 2.5D and 3D carved shapes.
We are perfectionists and we were hoping Mach4 was going to make the finish that much better than Mach3 thus reducing the microscope work.
I tried an example medallion that uses a .1mm Tip cutter with CV and found that it did not follow the same path as the G-Code, I may need to make some adjustments to the 0 to 179 Degrees in the CV settings.
Have you tried doing this with Mach4
Regards,
Mauri.
-
In regards to the tool path view, the only reason a machine can not follow the toolpath accurately in exact stop mode is if the step resolution is so poor that it can not possibly go to the requested position. Of course the display does not take into account machine flex or backlash....... which in the real world actually running parts can make huge differences.
What speeds you can set for different angles in the CV wizard is entirely dependant on 2 things. Your axis ability to accelerate and the tolerance you have to hold your tool path to. Its simple physics. Does your machine run like a pro-mod drag car, an Indy car or a bus? No mater how it performs, CV is a trade off. Nothing happens instantaneously. No matter how much accel and rigidity a machine has it cannot go around any corner (angle) without rounding it unless it stops at the end of one line and starts back in the direction of the next. End of story.
Now, what the CV wizard does is limit the feed rate to whatever you set it to for any given angle. It does not limit the feed rate in straight lines, only in corners (direction changes). So say your machine can take a 90 degree corner and only rounds it by about .010. If the tolerance you have to hold in that corner is .005 the .010 is not acceptable. So how fast your machine can take that 90 degree corner and still hold the .005 tolerance is the question. Unfortunately, your the only one that can answer that question. So, you have to do some testing to find out. When you do your testing I would do so in the worst case scenario (biggest tool, deepest cut in hardest material etc.). All of these considerations are trade offs as well. Maybe you use a 1.000 2 flute end mill to surface your aluminum table but most of your cutting will be with a .250 v cutter in styrofoam. So do you optimize the CV wizard to surface the table, do some v-carving in foam or somewhere in between? Lots of things to think about. This is why predefined (before the build begins) specifications are not optional if you hope to end up with a machine that will meet the end users demands.
-
Chaoticone,
Thanks for your reply.
Before I do machining I would like to see that the Tool in Toolpath G-Code displayed in Mach4 actually cuts on the same path.
Having produced many detailed cravings/engravings in 2.5D and 3D in Brass, we have optimized our milling machine as best we can and with Mach3 the results are not perfect but acceptable.
When running Mach4 and viewing the "Toolpath display" which is machine independent and has no short falls it should follow the path precisely if in "Exact Stop" and very close in CV mode if the CV settings are optimal.
That is what I am trying to accomplish, so until I can get a good path it is not much use in cutting actual maternal.
Any other assistance would be appreciated.
Regards,
Mauri.
-
What are your steps per set to for each axis? This will make a difference even if only in simulation mode.
Post up a picture of your whole Mach4 screen when it does not follow the path and a close up of a section that is off. Show us what your seeing.
-
Chaoticone,
I use a metric setup. 25.4mm to 1"
Counts per unit = 800 in mm or if in inches = 20320
Velocity Units/Minute = 1000 in mm or if in inches = 39.37
Acceleration Units/Sec^2 = 150 in mm or if in inches = 5.905512
As cutting brass in dry mode (continual Air Blast to cool) it does not require fast velocity or acceleration.
Give some time to set one up and I will today.
Regards,
Mauri.
-
Mauri I have not use M4 sinces the cv stuff was added, I am weighting to my pendent can be used with M4 before I move over, When that is working I will be as M4 is faster than M3 and works just that much better it's worth moving over, with the same trajectory engine M4 is better.
I got M4 to 0.001 +- .001 M3 is .002 +-002 after 1000 moves on any axis doing a Vcarve
-
Chaoticone,
Where does the CV feed rate by angle get stored once enter onto the CV Panel?
Is the any other quick way to set all 180 angles settings to say 10?
If the settings are Zero does that mean a complete stop at the end of an angle?
Regards,
Mauri.
-
The settings are saved in the profile.
If the settings are Zero does that mean a complete stop at the end of an angle?
Yup, if all the settings are set to 0 and CV feed rate is turned on and your running in CV mode it should run essentially the same as it would if running in exact stop mode.
-
Chaoticone,
Yes, I worked that one out.
A quick was to change the angle setting on all 180 is by editing the CV_Feedrate.mcs file.
-- grid:SetCellValue(i, 0, string.format("%.3f",feedrate))
grid:SetCellValue(i, 0, string.format("%.3f",10.000))
This for example will make them all 10.000.
Below are some Exact Stop us a 2.5D G-Code file made by Rhino5/madCAM5 using a 30Deg included angle with a .05mm Radius tip Cutter.
4 Display below of Mach4.
I also did the same with Mach3 Exact Stop, however the line display only joins up the dots that it makes and these dots do not represent all of the toolpath hence it looks as if it does not follow the path.
However all the dots are on the Toolpath line.
1 Display below.
On Mach4 I do not know how the program display is written so I cannot also say if the lines are correctly representing the Toolpath.
Regards,
Mauri
-
Chaoticone,
Max files was 4 so here is the last one.
Tomorrow I will do some CV Tests.
Regards,
Mauri.
-
Hi,
I have run some samples using CV and with the same 2.5D example on my previous mail related to Exact Stop.
In my previous runs although I had G61 set in the Configuration file, but I unfortunately had G64 in the code as I always used it in Mach3.
So I re-ran it and it does appear to be the same as CV 0. (see below)
The settings are all 180 angles at 0, 10, 50, 100, 400 & 1000.
The G-Code has X/Y at F400 and Z at F80 in simulation Mode with no Controller attached.
When you run it with all (180) angles at 1000 it seems to use 0 in the actual Mach4 program and Toolpath display.
Regards,
Mauri.
-
Hi,
The remaining CV runs all angles at 100, 400 and 1000.
I will try next using Mach4 with the Controller in bench mode (no Mill) and see what it does.
Regards,
Mauri.
-
Hi,
I apologize for any confusion and inaccuracies with my previous CV findings.
I have found that in a number of CV runs above, (in my mail) the CV was not applied correctly, hence a number were just the same or totally incorrect.
I found this out when I found some run times were the same when I made further tests.
To address this I decided to enter all my CV entries (180 angles) directly into the Machine.ini File.
The following JPG’s show finally, the correct display of each CV setting.
I ran CV 0,10,50,100,400,700 the G-Code has X/Y/Z in cutting mode all running at F400.
Each time the Machine.ini file was changes (CV Values) and Mach4 was run the CV table was checked to confirm that change.
The main reason for using CV is that we all do not have expensive HS Mills or Routers that have high tolerances and fast acceleration capabilities, so we require CV to reduce cutting time on long 2.5D and 3D runs and produce a suitable result.
Times for each run:
CV = 0 = 40:33.02mins best of all but not suitable for long machining runs as time would be excessive.
CV = 10 = 39.14.25mins very good but slow.
CV = 50 = 34:35.71mins not as good as 10 but could still be a reasonable cut.
CV = 100 = 29:48.70mins not suitable for fine carving/engraving 2.5D or 3D machining.
CV = 400 = 19:00.04mins very rough on angles.
CV = 700 = 19:04.07mins not sure why it took longer than CV=400 made no real difference as the max speed on X/Y/Z was F400.
Regards,
Mauri.
-
Hi,
Remaining 2 JPG's CV 400 & 700.
Regards,
Mauri.
-
Are you sure that Mach4 is displaying the actual toolpaths?
You posted an image of the Mach3 toolpath window earlier in the thread.
Mach3's toolpath is update 10x per second, and only shows the position that the machine is at when it updates. As such, it's not an accurate representation of the actual toolpath. The faster the feedrate, the less accurate the display is.
I'm just wondering if Mach4 is the same?
-
ger21,
Your right on Mach3, when it does dots they are spread apart and if you turn on lines they just join the same dot positions, so it does not represent the true accuracy of DV in Mach3.
I know that I get good results from Mach3 with 2.5D/3D and lines like tiny lettering.
With Mach4 if you blow up the image Toolpath and show it in 3D, you will see that it draws the line with on the G-Code line there is no jerky movement or jumps, so I feel sure it is a true representation.
Regards,
Mauri.
-
Hi,
If you want to improve the CV result in 2.5D and 3D Engraving/Carving you must have the same acceleration in the X/Y/Z axis.
I had a different one for the Z axis.
When I and made them all the same, then a CV 100 settings on all 180 Angles became acceptable.
The spacing between lines is .02mm with a .01mm tip cutter being used.
Next I will try it on small lettering.
Regards,
Mauri
-
Now, what the CV wizard does is limit the feed rate to whatever you set it to for any given angle. It does not limit the feed rate in straight lines, only in corners (direction changes). So say your machine can take a 90 degree corner and only rounds it by about .010. If the tolerance you have to hold in that corner is .005 the .010 is not acceptable. So how fast your machine can take that 90 degree corner and still hold the .005 tolerance is the question. Unfortunately, your the only one that can answer that question. So, you have to do some testing to find out. When you do your testing I would do so in the worst case scenario (biggest tool, deepest cut in hardest material etc.). All of these considerations are trade offs as well. Maybe you use a 1.000 2 flute end mill to surface your aluminum table but most of your cutting will be with a .250 v cutter in styrofoam. So do you optimize the CV wizard to surface the table, do some v-carving in foam or somewhere in between? Lots of things to think about. This is why predefined (before the build begins) specifications are not optional if you hope to end up with a machine that will meet the end users demands.
What is the relationship of feed rate in the CV wizard to the feed rate set by the gCode file? Is the output feed rate determined by the value entered into the CV wizard or is it limited by the feed rate set by the gCode? Or by whatever value is lesser?
Suppose I had a feed rate of 200 set for every angle >10 degrees, but the gCode is F120.
What would the feed rate of the tool be upon execution in a real world cut of 30 degrees?
Thanks!
53 Sparky
-
Is the output feed rate determined by the value entered into the CV wizard or is it limited by the feed rate set by the gCode? Or by whatever value is lesser?
Yes, whichever is less.