4th Axis on Forest CNC with CENTROID Controller

[smunzer8ZZFW]

I am working with a Techno CNC with a 4th axis that recently was upgraded with a Centroid Acorn controller. I have been tasked with getting this machine to work with a fusion post, but am having some trouble. I am testing wrapping  2d contour tool path but when I post the toolpath the operation fails and the .NC code can not be produced. I will attach below the prompts that come up when I try to post. I am wondering if this a problem with my tool paths, the post, or the machine configuration. 

[engineguy]

@smunzer8ZZFW 

Welcome to the Forum 🙂

First of all some more information is needed to check things out, number one, what is the configuration of your CNC Machine, is it a Rotary Axis that is mounted so it is in line with the X or Y axis?? A photo would be helpful.

Also what Fusion Post Processor are you trying to use, please attach a copy of the Post Processor .cps file then it can be checked for it`s configuration.

Meantime :-

See image below for a simple example of a 4th axis rotating around the X Axis cutting a Wrapped Contour.

If this is what you are asking for then try the attached example file and Centroid Post Processor, both work OK here, hope this is of some help, run the Simulation for the full program and Post the G Code 🙂 🙂

[smunzer8ZZFW]

Thank you for helping out, I will attach some photos of the machine below. I am using  2d contour wrapped around a cylinder.  @engineguy LINK TO CAM FILE  

[smunzer8ZZFW]

I also attached a link to the cam file below the pictures

[engineguy · Accepted solution]

@smunzer8ZZFW 

Well, the good news is that I have got it to work on some of your engraving, the main problem seems to be how the lettering is being selected and how it has been created, I think that you need to go back to your design and change a few things.

The lettering is such that some of the movements require a C Axis which you do not have so you the bad news is that it looks like you have a lot of work to do 😞 😞

For reference, it is best to not use a "Machine" unless you absolutely have to and the one that you have has no resemblance to your photo, also when uploading a file it becomes an f3z file instead of an f3d file if there is a machine in the setup and is just "clutter" for anyone else 🙂

I have managed to get one of your letters toolpathed and the attached modified Post Processor is outputting the correct B Axis code, hoep you have plenty of memory at the CNC control, that single letter is 180 lines of code, could get "heavy" 🙂 🙂 🙂

G Code file is attached and a modified Fusion file for you to work with 🙂

[smunzer8ZZFW]

Thank you so much, I really appreciate the time you have spent on this. I am still trying to figure out 4 axis machining. do  you have recommendation on how to get that lettering on the barrel? @engineguy 

[engineguy]

@smunzer8ZZFW 

You need to have everything properly aligned, see the attached file for an example, It works OK here and Post Processes the G Code OK 🙂 🙂 🙂

[smunzer8ZZFW]

I am having issues trying to post, I keep reeving the post failed message. The issue I am having is changing the plans in which the tool wants to cut in, even when I center the model the tool still want o come down in the X axis instead of the Z. I am just tryin to now get a simple rotorary tool path to work just to cut the contour of the barrel. 

[engineguy · Accepted solution]

@smunzer8ZZFW 

I don`t know what you are changing so not able to help with those, I have cleared out all the stuff in the file that is not needed and got it back to basics, it now works correctly and Posts Code correctly. Attached is a new Fusion file and a new version of the PP, again, test carefully.

A couple of tips, one keep everything as simple as  possible, a lot of what you are doing is not needed, second, when you are designing something and you are going to machine it then always try to create the design in the orientation that it will be machined in, for example, your CNC has a Z axis that goes up/down so the Z always points upwards, so always best to create in that orientation, saves moving/changing things later, it looks like you are working in design mode in the "Y axis up" orientation, go to your Preferences and change it to "Z axis up" so it is the same as your CNC machine.

If it is created on the axis in Design mode that is is to be machined on then it is a lot easier 🙂 🙂

Next, as you have found you can`t "Wrap" around a Taper, it has to be a circular face, if you make an extra body to wrap then the Engraving will not be the same depth, the letters will have a deeper cut at one end and will look pretty bad.

I suggest that you have that small section as a circular face as in the attached file and it will all be correct.

The only way that you could cut the letters correctly to the same even depth would be to use a 5 axis toolpath, as you do not have a 5th axis at your CNC then a small compromise is needed, make that section for the lettering a circular face.

Also, as you are working with Brass then you really need to Rough the majority of the material out with something like a 3D Adaptive toolpath, doing one side and then indexing 180 to Rough the second side, the Rotary is really only for finishing, cutting sideways at full depth with a small tool is not recommended 😞

[smunzer8ZZFW]

Okay I will keep working, again thank you so much for the time.