Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: ronniecruisin on October 06, 2015, 11:41:24 PM
-
Hi. All. Been out of action for a while and just getting back in to my CNC. I'm having a problem with the cut in Mach3. V cutting works fine with no problems but, in either Profile or Pocketing operations even though the simulation when saving the job in my drawing software shows perfectly square corners, when I cut the job it starts in a corner and cuts the other three corners with a radius, so the only square corner is the one it started at. Same thing happens when pocketing. From what I am able to find out the problem is at the Mach3 CNC end. The Art program is working perfectly. Does anybody know how to fix this??? Is it a parameter not set in Mach3??? The machine came with the program, but with very basic setup instructions. Regards to all ...Ron. ???
-
Hi. All. Between my last post, I found part of the answer to my problem.Saw an article Quick CNC. As in their page, changing the mode from Constant Velocity to Exact Stop fixed the problem. Only thing is now when cutting my little model window the machine cuts the straight lines in a smooth action , but the small curves it cuts in a small steps at a time speed. Should I change my motor and velocity settings to improve this??? In the quick article the settings they have are a fair bit faster than mine are set at. Mine is at 2000 for the X and Y. They are suggesting 4800 and 9600 for the X. Will this cause any problems??? I have noticed that the X speed is painfully slow, the way it is set now. Regards ...Ron.
-
Look at your gcode for any curved object, and you will probably see that instead of arcs the curve is represented / broken down to small combination
axis moves.
You set your max velocity and acceleration based testing such that axis movement will repeatable and without fault.
Also note that the feedrate in a program is user defined.
RICH
-
Thanks Rich. How do I change the curve to arcs you mention? I guess with the speed I can just experiment using the suggested ones Quick CNC have on their sheet.
-
How do I change the curve to arcs you mention
Don't know what CAD/CAM you are using, so it's done CAD first and CAM may recognizes the curve as an arc.
guess with the speed I can just experiment using the suggested ones Quick CNC
There are programs, charts, lot's of info on selecting the correct feedrate based on the material / tool / etc.
May want to learn how to rather than using some speed that may be meaningless for your setup.
RICH
-
When requesting assistance with a specific problem it's always helpful to give full details of any hardware and software involved.
That way you're not forcing those reading your post to help to make guesses or assumptions, with the added advantage that anyone with specific experience of your kit may recognize the issue and comment, rather than just assume they can't help and move on,
Regards,
Nick
-
Go to general config, and check "Stop CV on Angles>", and set it to 89. Then turn Constant Velocity mode back on.
-
Hi. All. Thank you all for your help. Gerry? You're a genius.! Your suggestion solved the problem. Basically my setup works well. I'm very happy with my Chinese machine. Only other minor issue I have and don't understand is, whatever I design in Artcam comes out half the size. I always have to double the scale in Mach3 for it to be the size I've drawn. Also I usually have to anything up to 4 times scale to get the depth of cut in the Z axis. Don't know if others have this issue. I've learned to live with it. Would be nice to know why it happens though. Thank you all for your help... Regards.. Ron.
-
You need to make sure your native units are correct, and y our steps/unit are set correctly.
One or the other, or both are wrong.
-
Hi. Gerry. Not sure what you mean. Native units are inch. Don't understand the rest. I just set it per instructions from Chinese, which is apparently pretty basic just to get it working.
-
Ronnie,
First off, you need to check the native units in mach to see that you are in inches.
If so, you need to make sure that you when you tell the machine to move one inch that the machine actually moves that distance. Chances are your machine configuration is set wrong. meaning your motor tuning needs to be configured to your machines hardware configuration. If your machine moves the correct distances, then you need to check which post processor you are using in artcam.
-
then you need to check which post processor you are using in artcam.
To ensure it's generating a G21 in the header for metric or a G20 for imperial?
As whatever you have Mach3 set to then a G21 or G20 command will override this?
-
Hi. All. Mach3 is showing G20 in the header. Native units set to inch. Motor tuning is steps per.2000 velocity.600 acceleration.4 step pulse and dir pulse.3. These settings are the same for all three axis. G.code inch is the only post processor I have found to work with this machine. It is a Stepmores. It is not listed in post processing options. Tried G.code mm. Machine travels excessive distances. Regards. Ronnie.
-
Those numbers are very wrong for a machine set up in inches, unless it's a very expensive, very high performance machine. Those are numbers you usually see for a machine set up in mm's. Since it's a chinese machine, that seems about right.
What are your steps/unit set to?
As for the post processor, you should be using a Mach3 post processor.
-
Hi. Gerry. Machine is v cutting a tree inlay at the moment, so will check when its finished. Where do I find that setting?
-
Right next to the other ones.
-
Assuming you mean in gen. Config. G20, G21 control lock DROs to setup units is not checked. And Distance mode is set to. Absolute and W mode is set to Inc.
-
No, the steps/unit is in the motor tuning.
-
Steps per.2000. Velocity 600. Accel. 4 G,s 0.0103607. Step pulse.3 Dir pulse 3 All three axis are the same. Spindle is different in step 1 and velocity 120
-
Ronnie, in artcam the model master post processors work well with mach3. cannot remember if there is an inch one or not.
Have you checked to see if your machine is moving the correct distances?
Lay a ruler on the table. Zero the X or Y axis over an inch mark. Work cordinates to Zero. Use the MDI line. G0 x 1 press enter, did the X axis move from one inch line to the next? i will bet money that it only moved under half the distance.
-
Hi. Fixxitt. Yes. You are correct. It does move only half the distance. Everything I draw, I have to double the scale on Mach3. I have also used Aspire. Same thing. G code inch works. I've tried using a few post processors. Not sure if I've tried the one you mention. The machine works just fine. Would be nice to have this right though. Regards... Ronnie
-
Ronnie,
its moving half the distance because Mach3 is not configured to your machine correctly. It has nothing to do with any type of cam/post processor issue. It is all in mach3.
Go to CONFIG>MOTOR TUNING. You will be in the X axis motor movement profile. The bottom left corner is the "STEPS PER" box. This is where you "TELL" mach 3 how many steps it needs to make to move one UNIT. Be it inches or MM`s. So if you tell your machine to move 1 inch, and it moves less then one inch, then your STEPS PER is to small. If it moves more then the steps per is to big.
So right now if your machine is moving half of what it should, double the steps per. YOU MUST CLICK THE "SAVE AXIS SETTINGS" BUTTON ON EACH AXIS BEFORE MOVING TO THE NEXT ONE.
Here are the steps. It can be a little tricky if you do not rezero the work coordinates after a motor tuning change.
Get a ruler, place it on the table along the X axis. lower your spindle/tool over an inch mark on the ruler. Zero the work coordinates for X
Use the MDI line and type G0 x1 and press enter. See how far it has moved. You want it to go to the next inch mark
In the MDI line again type x0 and press enter. This takes you back to the starting point.
Config> Motor tuning> x axis Adjust the steps per higher or lower by guestimation on have for the x axis moved.
Click the SAVE AXIS SETTINGS BUTTON
Click Ok to get back to the main mach screen.
STOP!!!!!!!!
LOOK AT THE X AXIS WORK CORDINATES!!!!!!!! They are no longer set to zero. The change of the steps per caused them to change.
Zero the work coordinates for the X axis and replete the MDI moves.
Dial it in. If you forget to rezero the X axis after a change. Telling it to move to X 1 will give you a funky rotation that could throw you into a mind loop.
I know it sounds like a crap ton of complicated stuff, but it really is not.
-
Thanks fixxitt. Very nice of you to spell it out for me. I am in the middle of a project that I need for the weekend, so I'll wait till the job is finished, and then follow your instructions. I'll let you know how it goes. Thanks again to all who have helped. Regards... Ronnie.
-
I dont use the standard mach 3 screenset, so I had forgotten about this until yesterday, but go into the settings screen, very bottom left is AXIS CALIBRATION "Set Steps per unit" button. Follow the instructions. Make sure you can accurately measure movements.
-
Thanks Fixxitt. I assume you mean follow the instructions on that page. Had a look at the first step, where it askes how far I want to move the x axis. Is 1 one inch? For instance? I'm just not game to change anything till I've finished cutting my stuff for the weekend. Would be a disaster if I couldn't finish it. I'll have a go when that's done. Regards... Ronnie.
-
Ronnie, the box that asks how far you want to move is the native units. so if your setup in inches it will be an inches move. So if you told it you wanted to move 5 inches or 1. It will use the motor tuning config to move what it "knows to be that value. make sure you Zero that axis first. Then you measure how far the machine actually moved and put that in the next box that pops up. It will calculate the steps per. So being able to accurately measure the movement is a plus.
-
Oh. Ok. That sounds good. I'll give it a go and let you know what happens. Regards... Ronnie.
-
Hi. All. Fixxitt. I haven't done that adjustment yet. Still try to get a few things done. Taking longer that expected. Even though my other issue seemed to be solved and was working fine, it's come Back again. Cutting a new small arched v cut profile for model windows and the machine is cutting a few rounded corners here and there. The tick stop cv on angles 89 degrees worked for my other windows. I notice that in the same cv control box next to the above mentioned parameter there is another one.cv tolerance. This is not ticked but has a figure of 180 units. Should this be a different figure? The machine works fine on everything else I do on it. This has got me puzzled. Regards Ronnie.
-
The best way to get rid of rounded corners is to increase the acceleration settings, IF your machines is capable of accelerating faster.
Otherwise, I'd try playing with the CV angle setting, and wouldn't bother with any of the other CV settigns, unless you want to do several hours of careful testing to find out what works best for your machine.
Here's a document that explains what the CV settings do.
http://www.machsupport.com/wp-content/uploads/2013/02/Mach3_CVSettings_v2.pdf
-
Thanks Gerry. I'll try your suggestion and see how it goes. Its weird though. The fix you gave me last time worked perfectly. This is the same type of drawing as then all done the same way, but now its playing up. Anyway try again. Thank you. Regards... Ronnie.