Screw question & funky movement

[Serb]

For about a year and a half I'm running the beginners setup with a Acme 1/2-10 single start screws and I'm getting tired of the lack of precision and the overall play within the machine movement. I's a fine setup for the money invested but I'm stepping up. I'm fixing to get rid of all the MDF except the table that is solid and bolted to a steel structure and go with real linear bearings. I followed the previous post talking about the issues with 2 & 5 start screws trying to find out what would be good precision screws without going bankrupt so I wanted to create a separate post just dealing with precision instead of speed.

My second issue would be the movement of the machine when it's cutting a curve or a circular pattern. This does not happen with small radius patterns but on the larger ones the machine does not follow the curve cut in a smooth motion and it travels in waves as it receives the information from Mach3. It does not have the constant velocity on curved patterns (diagonal straight cuts are fine) and I know there is a setting for CV in Mach3 but if I set it on then my sharp corners come up rounded.

[ger21]

Originally Posted by Serb For about a year and a half I'm running the beginners setup with a Acme 1/2-10 single start screws and I'm getting tired of the lack of precision and the overall play within the machine movement.

Not sure why you're seeing a lack of precision? 1/2-10 acme should be very precise. I use it on my Z axis and jog in .002 increments to set my zero point. But since you mentioned "play", it sounds like you have a bit of backlash, which can also effect repeatability. Simply upgrading to anti-backlash nuts should fix your problem, provided the screws are securely mounted, and not moving.

I followed the previous post talking about the issues with 2 & 5 start screws trying to find out what would be good precision screws without going bankrupt so I wanted to create a separate post just dealing with precision instead of speed.

The faster you go, the less resolution you'll have. 1/2-8 2 start will give you twice the resolution of 1/2-10 5 start. Twice as many steps/inch. And, depending on motors and drives, 1/2-8 2 start is still capable of giving you up to 150-200ipm speeds.

My second issue would be the movement of the machine when it's cutting a curve or a circular pattern. This does not happen with small radius patterns but on the larger ones the machine does not follow the curve cut in a smooth motion and it travels in waves as it receives the information from Mach3. It does not have the constant velocity on curved patterns (diagonal straight cuts are fine) and I know there is a setting for CV in Mach3 but if I set it on then my sharp corners come up rounded.

If you have CV turned off, and you circles start and stop, it sounds like the g-code is made up of multiple arcs for each circle, or the circle is made up of multiple straight lines. Ideally you'd want it to be a single G2 or G3 line of code.

One thing you can try with CV mode. Go to the settings page, and make sure CV distance and CV Feedrate are turned OFF. Then, go to General Config and uncheck all the CV settings except the last one. "Stop CV on Angles>". Check this and set it to 89°.

[Serb]

Not sure why you're seeing a lack of precision? 1/2-10 acme should be very precise. I use it on my Z axis and jog in .002 increments to set my zero point. But since you mentioned "play", it sounds like you have a bit of backlash, which can also effect repeatability. Simply upgrading to anti-backlash nuts should fix your problem, provided the screws are securely mounted, and not moving.

I did notice that when jogging the Z in step increments it can be very precise. I will upgrade the anti-backlash nuts and I also need to try to replace the Enco lovejoys' rubber connectors with the ones Joe did in his DXF files or should I just go with the solids?

The faster you go, the less resolution you'll have. 1/2-8 2 start will give you twice the resolution of 1/2-10 5 start. Twice as many steps/inch. And, depending on motors and drives, 1/2-8 2 start is still capable of giving you up to 150-200ipm speeds.

What would be the advantage of going from 1 start to a 2 start screw, is it just the speed?

If you have CV turned off, and you circles start and stop, it sounds like the g-code is made up of multiple arcs for each circle, or the circle is made up of multiple straight lines. Ideally you'd want it to be a single G2 or G3 line of code.

I use ArtCam to generate the toolpaths and most of the time I do the drawings in Corel or AutoCad and open the files in DXF format. To save the toolpaths I use Mach2(Inch) post processor and the machine has a HobbyCNC Pro Board. Is there a different post processor that I can use to create a single line of code or some other way of doing it?

Thanks G for all the info and for saving me $ I don't have.

[ger21]

What would be the advantage of going from 1 start to a 2 start screw, is it just the speed?

Basically, yes. It'll double your speed, and cut the resolution in half. But it will still have more resolution than you'll need.

I use ArtCam to generate the toolpaths and most of the time I do the drawings in Corel or AutoCad and open the files in DXF format. To save the toolpaths I use Mach2(Inch) post processor and the machine has a HobbyCNC Pro Board. Is there a different post processor that I can use to create a single line of code or some other way of doing it?

Draw a single circle, and post the g-code here. If you can, also post the post processor you're using. And what version of AutoCAD?

Also, draw a circle in Corel and upload the .dxf here too.

[ger21]

Try running this code and see if it runs smoother? It doesn't go below Z=0, so it shouldn't cut anything.

[Serb]

Originally Posted by ger21 Draw a single circle, and post the g-code here. If you can, also post the post processor you're using. And what version of AutoCAD? Also, draw a circle in Corel and upload the .dxf here too.

I drew a simple circle and an arched with a closed line between the endpoints so here are the DXF files from AutoCad 2009 (saved as a 2004 version) and Corel (also save as a 2004 Version) and the corresponding toolpaths. There's also a post processor file from Artcam that I did the toolpaths with.

[ger21]

two problems. One, that ArtCAM Post will not output G2/G3 arcs. Not sure if it can be changed to do arcs.

Second, the circle from corel is actually an ellipse, and the arc is a spline. typically, both of those types of entities will give you straight segments, and not G2/G3 arcs.

You might want to try my AutoCAD macro to export g-code from AutoCAD. You need to convert arcs to polylines, but circles are fine. It's quick and easy once you get the hang of it. http://www.cnczone.com/forums/showpo...&postcount=196

[Serb]

Is there another post processor that will work in ArtCam and running Mach3? I don't mind using AutoCad but how would it work if I'm cutting relief objects?

[ger21]

If your cutting reliefs, you'll always get G1 moves, so a different post processor won't matter.

[Serb]

Originally Posted by ger21 If your cutting reliefs, you'll always get G1 moves, so a different post processor won't matter.

You are correct, I don't know what I was thinking when I asked that question.

Usually the relief objects get a rough cut and I use the same bit to do the exterior perimeter cut and the two toolpaths are saved under a single g-code file since it's the same bit.

I was testing different post processors and Mach3 Arc and G-Code Arc were able to produce a G2 even from a Corel file. It would split a circle into 4 sections (even the AutoCad circle) and the arc with a single radius would be done with a single line of code. I did another arc looking thing but it was more like a half of an oval and it did split it into segments since there wasn't a single radius there.

Thanks for leading me in a right direction