Recent changes to Mach3 post processor

[jameswyatthopkins]

Hello everyone,

  Recently after a series of updates to Fusion, I have been experiencing some difficult changes to the Mach3 post processor. It seems that the tool change command has changed to tool number first and M6 second. Mach3 does not like this order and it is a pain to change all the tool change blocks. 

   Could it be possible to get this corrected and set it permanent so it would not fluctuate all around. Would seem to be good to let the post stay the same after it is stable. 

Thanks 

[johnswetz1982]

The installed post get overwritten every time fusion gets updated. If you have a working or modified post you need to save it to your cloud settings or have a copy someplace that does not get overwritten whenever there is an update.

[johnswetz1982 · Accepted solution]

I am trying to learn more about the post editing, I think what you want would be to change;

if (properties.useM6) {

writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));

to

if (properties.useM6) {

writeBlock( mFormat.format(6), "T" + toolFormat.format(tool.number));

[jameswyatthopkins]

I understand that the posts are overwritten every update but it would seem they would stay the same. 

[seth.madore]

Hmm. And it's been M6 T1 in prior versions? I've got a couple older versions and I'm not seeing that behavior...

[jameswyatthopkins]

I had a friend just a couple of weeks ago also ask me about this same problem, it seems the same condition is still causing the tool code to be posted out of sequence for Mach 3. I have corrected my post and saved it to my cloud but people who are not aware of this and not used to correcting or altering post processors it is a problem I'm sure.

[engineguy]

@jameswyatthopkins 

By all means go ahead and alter the PP, however I have to disagree with you and agree with @seth.madore regarding the correct sequence for a tool change in Mach3, or even Mach2 and Mach4 they have always been T** M6. if your version of Mach3 won`t accept that command then I think you need to maybe change the version of Mach3 you are using, some versions are notoriously unstable and "buggy", what version are you using? Is it the last "stable" version??

Over the years I have built/retro-fitted/modified more than a dozen CNC Mills and Lathes and 1 Router and 1 Laser using various Mach3/4 setups, some for myself and some for others and I have never seen any Post Processor that I have used with several different CadCAM softwares, (FeatureCAM, BobCAD-CAM, MasterCAM) in every one of them the Post Processor for Mach3 has always output Tool first and then tool change command M6 (or M06). They are all very mature CadCAM softwares, years and years ahead of Fusion 360, a good guide to how mature and stable a CadCAM software is to go to the Forums (CNC Zone, their Forums etc, etc) and the ones that have very little posting are the ones that work well and no body needs to Post!!

Fusion 360 is still quite young (Relatively speaking) so we constantly have things that did work OK getting "broken" because the developers have done something somewhere else that has affected it!!

Mach3 is actually Fanuc based and that is the way it has been done for many, many years and it does work!

I am not having a go at you, but to be saying that the Fusion 360 Mach3 PP is wrong is actually wrong, it may  not be perfect but there again nothing about Mach3 is or ever will be, have you considered moving to Mach4 ? I have used it on a small 3 axis VMC and it does work way better than Mach3 🙂 🙂 🙂

Regards

Rob

[daniel_lyall]

I just check in 3 different cam programs they all have tool then tool change these are one I have been using for years.

@jameswyatthopkins  What do you have tool change set to in general config?

[jameswyatthopkins]

My Mach3 software does not accept tool number first. M6 must be first then tool number.

[jameswyatthopkins]

It is funny how this just started happening, I am not the only one to have this problem I know of four other friends of mine that have noticed this change. I actually use MSM to controle my mil and it requires the latest version of Mach3.

[daniel_lyall]

Locking on their forum they are using T# then M6 I found a post where art tried T# M6 and M6 T#.

Just put in T1 M6 into the MDI and hit enter then try M6 T2 they both should work.

[engineguy]

@daniel_lyall 

Daniel, I have loaded the same code from Fusion Mach3 Post Processor into 3 different Mach3 setups, a standard 4 axis, a modified 6 axis and an MSM setup, they all accept both the T** M6 or the M6 T** quite happily and run the code without any errors 🙂

As can be seen from the images above there are no issues at all with any of the setups, I have done two images of the MSM showing both ways accepted without issue 🙂 🙂

Mach3 version used on all setups is R3.043.062 which I believe is the latest download available.

Regards

Rob