Vectric 2DCut and Mach3

[GoCreateParticipant @gocreate]

G code mess

[GoCreateParticipant @gocreate]

Hi

I am just starting out on cnc and trying to use 2DCut to generate G code for Mach3.

I have tried several projects, some from dxf files and others drawn in 2Dcut but all with the same result.

 

All seems well in the 2DCut programme, the preview works OK. It saves the Gcode as a text file, when I load this into Mach3 there are masses of circular tool paths As can be seen in the above screen shot.. The actual tool paths wanted are in there (red lines) but obviously something is a miss.

 

Anyone using Vectric 2DCut and Mach3? Any ideas of what the problem is.

 

Incidentally I have used Meshcam to machine some test 3D shapes without any problem so I am sure this is to do with how 2DCut is processing the Gcode.

 

Any help appreciated.

 

By the way, I have tried to register with the Vectric Forum but it yells me my IP address is not permitted, hmm I have paid my money now.

 

Thanks

Nigel

 

PS. the profile I am trying to machine in this case is that of a Jaguar (cat). I will screen shot fron Vetric to my album to show the intended result.

Edited By tractionengine42 on 09/10/2011 17:50:05

Edited By tractionengine42 on 09/10/2011 17:50:43

[GoCreateParticipant @gocreate]

Here is a Preview from Vectric showing what the expected result should be.

 

Cheers.

 

Nigel

[Jim GuthrieParticipant @jimguthrie82658]

Nigel,

 

Have you got the post processor definitely set to Mach2/3 mm (or inch)? The choice is in the drop box immediately above the Save Toolpaths button. I’ve been using Cut2D with Mach 3 for the past year and it has always worked well with no interface problems with Mach3 on a KX1 mill.

 

Jim.

[John Stevenson 1Participant @johnstevenson1]

Nigel,

 

I wish I had a pound for every time I have answered this question.

In Mach3 go to the Config menu on the top line, select General Config and in second block from the left 2 down ? there are two radio buttons for Arcs.

You will have absolute selected, change this to incremental, close the program, reopen and jobs a good un.

 

As Jim says you need the correct post processor.

Edited By John Stevenson on 09/10/2011 18:54:09

[John Stevenson 1Participant @johnstevenson1]

Something else I have thought of.

Mach as setup out the box is mainly imperial. If your code has G20 at the start it will work in imperial or G21 makes it work with metric but there are other underlying parameters that force some imperial moves.

 

When Mach load up it reads an XML file that is saved from your last settings and if you don’t tune these setting you have a miss matched set.

 

For the metric guys go to Config > General Config and roughly central is a line called Initialisation String.

Not sure what the default is as I don’t have a standard program on my machine but I think it’s something like G80 F6.0 this tells the program on load up to cancel any drilling cycles and run at a default feed rate of 6 inches per minute.

 

If you are working in metric this is then read as 6mm per minute which is an absolute crawl.

 

A metric users string need to have the following

G21 G40 G49 G80 G91.1 F125

 

This will put it into metric mode, cancel tool length offsets, cancel tool offsets, cancel drilling cycles, put arcs into incremental mode and run at 125mm per minute which is a nice default speed.

 

Again close the program, reopen it and you are now in full metric mode.

 

John S.

Edited By John Stevenson on 09/10/2011 19:07:57

[GoCreateParticipant @gocreate]

Hi Guys

 

Jim, yes I saved under mach2/3 mm

 

John, I made the config changes you stated and it’s now working perfect.

 

I obviously need to learn more about config options.

 

Thanks so much, I had not expected such a quick and easy solution, that’s the power of forum’s, superb community support.

 

Cheers

Nigel

 

 

 

 

 

 

[GoCreateParticipant @gocreate]

Hi john

Your second post must have arrived as I was making my reply.

 

Thanks for the additional info. Currently I am dedicated to metric so will have a look at what your saying.

 

I was thinking of having a metric and imperial configurtion and loading either via Mach3 loader. I assume that should work OK?

 

I was just wondering, the setting I have just changed from absolute to incrfemental, is there likely to be a circumstance where I would need to change it back?

 

 

Thanks again

Nigel

 

 

[GoCreateParticipant @gocreate]

Hi John

BTW, I also wish you had a pound for every time you have answerd my question, your worth every penny.

 

Thanks again

 

Nigel

[John Stevenson 1Participant @johnstevenson1]

Bollocks, just done a big reply direct into the reply box and then got a message saying you must paste from word ?

 

Then deleted everything

 

WTF ???

Not using word.

 

This has got to be the crappiest web site this side of Russia

Edited By John Stevenson on 09/10/2011 20:33:31

[GoCreateParticipant @gocreate]

Hi John

Sorry to hear your frustration, it’s such a waste of valuable time when these things happen.

 

You will have gathered I am very new to cnc but learning fast. Just this post has shown me allot by pointing me in the right direction.

 

My startup string only has G80 so I will add the others you mention. I checked the gcode on the programme and the codes you mention are at the beginning so I guess vectric is doing a good job there and all should be safe.

 

I am keeping my feed rates very low until I feel a bit more confident.

 

Cheers

Nigel

[GoCreateParticipant @gocreate]

Hi

I don’t usually look at a manual until I have broken something, so I thought this time I would get ahead of myself.

 

The mach 3 manual actually explains very well what John has advised and I can now begin to understand this absolute and incremental stuff.

 

This website seems very good if your just learning G-code, click on a g code and you can walk through a visual illustration of what the Gcode is doing. looks good to me anyway.

 

Learn G Code

 

Another useful G code referance

 

Nigel

Edited By tractionengine42 on 10/10/2011 10:44:03

[Steve WithnellParticipant @stevewithnell34426]

 

 

Edited By Steve Withnell on 10/10/2011 22:39:06

Edited By Steve Withnell on 10/10/2011 22:39:45

 

 

Edited By Steve Withnell on 10/10/2011 22:40:38

[John Stevenson 1Participant @johnstevenson1]

 

 

 

 

Come on Steve – spit it out

John S.

[blowlampParticipant @blowlamp]

It’s, it’s, it’s…….

………It’s like the sneeze that never comes.

 

 

Martin.

[Steve WithnellParticipant @stevewithnell34426]

Polite words on how crap this forum software is failed me…

 

The ones I had in mind would have been deleted…

 

But because the software is junk – guess what – there is no delete!

 

[GoCreateParticipant @gocreate]

Result

1st Vectric 2DCut engrave

2nd Vectric 2DCut – pocket mill
Allchin Front Wheel Hub

Milling cutter 0.2mm x 20 deg engraving cutter, 8000 rpm, 200mm/min max.

23500 lines of code.

A liitle more conventional machine work to do then just need to infill with red enamel and polish

 

 

Nigel

 

Edited By tractionengine42 on 12/10/2011 14:19:17

Edited By tractionengine42 on 12/10/2011 14:26:21

[John Stevenson 1Participant @johnstevenson1]

I thought there was only one G in England ?

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Got ya

John S.

[GoCreateParticipant @gocreate]

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Ha Ha.

You did get me, for a moment I thought it was “back to the CNC” or should that be drawing board

 

 

Edited By tractionengine42 on 12/10/2011 15:35:26

Edited By tractionengine42 on 12/10/2011 15:36:45

[IanHParticipant @ianh]

Hi Nigel,

I am a Cut2D Mach3 user – recently graduated to BobCad Cam for 3D work. How did you generate the .dxf file for the brass hub caps (or whatever they are)? Cut2D has very limited cad capability so I tend to bring .dxf files from Autocad into Cut2D then add the text in Cut2D but I wasn’t aware you could fit text to a curve. Are you generating the text elsewhere?

Ian

[GoCreateParticipant @gocreate]

Hi ian

I use autodesk inventor for my work so I am able to use this for creating quite a few dxf and stl files for my cnc work. This software allows you to fit text to a curve.

 

If I can help you with a particular requirement send me a PM and I will see what I can do.

 

Nigel

[Author]

Posts