[Ranol]

Hello,
One year ago I decided to built the first laser machine in Greece.
The laser source is from Rofin and the model is SCx30w.
I made all the construction. The working table is 2100 * 2500 mm and there are 3 axis offcourse.
Unfortunately for me, Greece is a few years back in technology and they do not know lot of things about CNC and laser machines.
Anyway, the movement is from Bosch rexforth but not the servo drives but the railways. The servo motors are from SEM if you know it and the other part which goes with the servo is from Atlanta company. Anyway I dont think that all this might help for the problem I have now.
Everything is ok, but the main problem is the CNC. What I mean is, my PLC or controller if you say so, is ECKELMANN and the servo drives is from METRONIX.
The first problem that I have is that when the laser cuts a circle or a rectangle there are PERFECT!!!!! BUT! when I have a curve or an arc or an spline or anything else except circle and lines, the cutting quality is very bad! it cuts small lines, I dont know if you understand what I am trying to say for eg. when we have the letter S for example in the place that there are curves it will cut with the direction of a curve but when you look at it there are many big or small lines. I believe that the problem is from G code, but nobody knows.
My father built this machine and I am his daughter and Im so sad that we cannot figure this out. I am reading lots of things and Im trying to help him because the people who made the CNC installation they dont have a clue!!!
Anyway, is anyone have any idea about the problem I said? Offcourse this is not just one problem we have lots of problems.
I'll try to show you some pictures of the machine.
When we started making this machine we didn't thought it would be so difficult on the electronics part. Also the software is a huge matter too. We use SheetCam, it is ok but it is not enough for us.
The laser is working but not on the right way.

I will wait for any idea or any question that you might have.
CNC ZONE is my last hope!
Thank you,
Alice

[jpgdesigns]

Ranol,

Splines and curves typically get broken down into the most basic elements - lines and arcs... most of the time little lines.

I have not used sheetcam so I can't really speak about it, but have programmed code for and opperated gantry style cutting machines for most of my life.

This is what I would suggest to start.

Since you can cut circles and rectangles "perfect" this is due to the fact that circles are typically made up of 1 line of g-code and a rectangle is typically made of 4 point to point moves in g-code. I woud suggest a little test, to see if its more a controller problem or a g-code problem.

First, make a g-code program for a rectangle use no less that 4 little lines to make each side of the 4 sides. The controller should treat this code as if it were one line from side start point to side end point. If it accel/deccel for each segment of the 4 that makeup each side, that is a controller problem and should be resolved first.

If the machine cuts the rectangle to the quality you expect then I would look to the software I am using to creat the geometry and g-code.

I would start with the post-processor software, there may be a setting to adjust the tollorance when converting splines and curves to tool path.

If not there then maybe look at the CAD or Art package that is creating the original geometry. It may allow you to "convert" the curves to lines and arcs that will give you the quality you are looking for.

Hope this helps...

James G.

[ger21]

As the previous poster said, the straight segments are probably coming from your design package. What are you using? Can you post the .dxf your taking into SheetCAM that has the problem? You might also want to contact Les, the author of SheetCAM.

[Ranol]

Thank you jpgdesigns for your information, I will make a test with the rectangle tomorrow morning. But I think, if I understood correct with the word "accel/deccel", that in each segment does that. accel means the speed is increasing?

Ger21 I use Autocad for the drawings and afterwards I go to the Sheetcam and the only that I do is to import the .dxf file and push the button for the post processor. I will post the .dxf file tomorrow.

I know that in all drawings everything is lines but other straight other curves.
I tried to add lots of segments to the drawing and the result was to make more and more lines but smaller offcourse. Tomorrow I will post two photos with the segments so you can see what I mean.

I will contact with Les, maybe he has an idea about it.

As I have seen in other laser systems, the software has an option "smooth" usually. I don't know if I need something like that.

I will have more news tomorrow
Thank you very much for your replies.

[ger21]

How are you doing text in AutoCAD?

[Ranol]

Ger21 I don't do text in Autocad, I just do the drawing and then I go to Sheetcam where it produces the g code through the post processor. After I can do some changes if I want with the notepad. The format that goes out from Post processor is in .din . Hope I answered to your question.

[ger21]

Not really. What are you creating the text with?

[Ranol]

oh my Im so sorry. Well I still don't get your question sorry..
could you give me an example?

[ger21]

You said you had problems with text not being smooth. What software is the text being created in, if not AutoCAD?

[Ranol]

Oh alright Now it is clear. Well, I made the drawing in Corel and then I saved it in .plt format and then I went in Sheetcam and made the rest.
But It is not only with letters, but generally with curves and arcs. Anything that it is not a circle or a rectangle.

[ger21]

This might help you. http://www.candcnc.com/DXFToolDetails.htm

[Ranol]

oh thank you so much. I will make the tests tomorrow morning cause today is sunday and I didn't go to work.
I will post some photos
Thank you ger21

[hkxy]

I suspected that,Software and pulse match,
As well as transmission gap.
Whether can watch your picture,If you keep secret.

[jpgdesigns]

Ranol,

Since you are using AutoCAD, I assume you are exporting DXF in R12 format.

R12 converts splines to plines straight segments.

Also, if your machine is speeding up and slowing down for each little segment that is a problem. The controller should "look-ahead" at the code and move smoothly.

Also, I think it would be better to DXF out of Corel.

Hope this helps.

James G.

[Ranol]

jpgdesigns,

well I dont usually export in r12 format but in a newer format and this might be a problem. I will search for the "look-ahead" in my g-code.
ger21 gave me a really good link and I wrote to this company, I downloaded the demo version, I tried to make a test but I was a bit confused.

The problem I have when I export from corel to dxf files is that when I go to Sheetcam, Sheetcam cannot see the drawing!! and it is so wierd! When I export in .plt format then Sheetcam imports the drawing correct!
I tried several times to solve it but I really don't know what is happening!

Maybe I have to contact with Sheetcam.

However, thank you jpgdesigns for your information, I'll try it tomorrow.

[ger21]

You might also try hpgl from corel.

[Ranol]

ger21 yes I can only import files from corel to sheetcam through hpgl and plt if I remember correct. I cannot dxf at all and I think that .dxf format is better than .hpgl or .plt .

[Torchhead]

There are problems with the native DXF export from Corel. It does not do curves and uses line segments. The segments from DXF are pretty course. HPGL does the same thing but the segments are smaller.

There are two issues here. One is the segmented art. The other is what the motion software does with the segment file. Good control software will look ahead at the toolpath and "smooth" the segments. You do get the jerky start and stop with each segment.

Go to www.machsupport.com and download the manual for MACH2/3. Study the part on "Constant Velocity" (CV). If is the segment smoothing portion of the software. If your motor drive system takes Step & Dir signals to drive the motors you can use MACH3 from a PC and parallel port.

I saw you joined my support site (CandCNCSupport). Ask any CNC questions you want or questions about CorelDraw, SheetCAM of the DXFTool. I'll do my best to answer them.

The DXFTool for Corel translates the arc and curves into splines (instead of line segments) and SheetCAM will import it directly. The current version of DXFTool requires that you convert text to curves in Corel prior to export but we have a new version that will be posted early this week that will resolve that issue. You will be able to leave your text objects as text and come back and make any changes to the text and still get full arcs and curves into the DXF.