[hkenuam]

So I finally got around to trying some 4th Axis wrapping in Bobcad V23. However, when I ran it on the machine (a Milltronics w/Centurion 6 control), the generated code executed one line at a time. I tried some engraving on some round stock and you can literally see in the engraving, each command executed. This cause the A axis to continually stop/break pulse air (HAAS). While others thought it generated a rather interesting affect, it couldn’t be more wrong in my mind. It should have been a smooth cutting action.

I think it has to do with the setting of absolute arcs but not sure. Does this make sense?

Attached is the program.

Thanks in advance

[HuFlungDung]

It doesn't really matter what kind of arc format you use, wrapped arcs will be interpolated line segments, and you kind of have to use fairly short interpolation for it to look 'rounded' and curvy.

You should also program an M11 on Haas, to release the brake before you begin engraving, so the machine itself does not have to stop and cycle the brake between moves. My experience is with a Haas rotary on a Haas mill, with 4th axis prewired, so I'm not sure how that works on your setup. You might have some other means to release the brake if you are running the Haas control box, which I have no experience with.

[hkenuam]

Would you happen to know how to instruct Bobcad to program an M11 besides adding it manually?

[BurrMan]

You can hard code it into a post.. Open MillEditPost.exe from the root of the bobcad installation and select your post.. Then look at the code blocks tab..



Note the values in quotes are "hard coded" values and output as typed.. Pay attention to the "standard start of program" and the 2 "tool change" blocks.

[mcphill]

You can do what BurrMan and save it as a new name, and use it for 4th axis work only. That way the code would not be put in when you do 3 axis work (if you care...).

[hkenuam]

So when I open the file, mine doesn't display anything on the left, however, I can still click on each of them. Wierd. But anyway attached is the change that I would need to make. Does it look correct?

Thanks again!

[The Engine Guy]

So when I open the file, mine doesn't display anything on the left, however, I can still click on each of them. Wierd. But anyway attached is the change that I would need to make. Does it look correct?

Thanks again!

What you have done will produce an M11 hard coded into every G code generated, whether it is in the right place for your machine I wouldn`t know

You need to open your Post Processor in Notepad and scroll down to the bottom and you will most likely find program blocks that are called up by scripting, that`s why you don`t see your "tree" in the post editor.

Delete all the lines that have 2*** numbers like these:-

2001. Program Block 1.

2002. Program Block 2.

2003. Program Block 3.

2004. Program Block 4.

2005. Program Block 5.

2006. Program Block 6.

and you should be able to see the "tree" on the left.

Alternatively if you want to keep that stuff then just use Notepad to edit your Post Processor, just make your changes and click save, job done.

Regards
Rob
:rainfro::rainfro::rainfro:
.

[BurrMan]

That will work.. That line will put the M11 on a new line all by itself at rthe start of each new operation... Be sure to review the toolchange positions and what your machine will do just before, and at the begining of each toolchange. Like maybe you want to apply the brake, make the toolchange, then turn the brake off again.. But I dont know how a Haas works.

And as the General p[oints out, editing out the scripting blocks from the post processor will have the MillEditPost application work again.. It was written before the scripting was added, and doesnt know how to deal with the new blocks properly.