Hi All,

We have recently purchased a used Biesse Klever 1530 5x10 flatbed CNC to boost our production capabilities. Our company makes custom pieces and artwork so most of what we do is wayyy beyond the Biesseworks software that came with the machine.

We have been using Fusion 360 for years, so our hope was to create the models and tool-paths there and export to Biesseworks to run the machine.

The CIX post-processor we got seems to work, but we get errors in Biesseworks and sometimes geometry just dissapears. I also can't seem to find a way to create tool paths for gang drilling within Fusion 360. Our machine has a 5-drill block on the X-axis.

Advice from Biesse is to try Mastercam or Alphacam (both = +$$$) since they've never heard of Fusion 360.

Autodesk hasn't been much help either.

Am I trying to mix oil and water here?

We are using Fusion360 as well as other cabinet software to run our CNC machines including a 5x12 Onsrud Flatbed among other machines. Fusion is quite good and for more complex stuff it has been our goto. complex 3D toolpaths have been done without issues. We have had to drip feed these larger programs into the Onsrud because it only has a finite memory.

For the multi drill block we have thus far only used it inside our cabinet software and it works fine that way. I am quite sure that there is someone who could make fusion360 use the drill block but at this point we are not using it for that. Lately we have been moving to doing a lot of 3D modeling of cabinetry in our Fusion360 because it allows a lot more flexibility of design albeit with some difference in design time. A lot of what makes dedicated cabinet software so capable is the ability to change things globally or per cabinet on the fly and not have to move a lot of bodies around etc. This of course can be accomplished in Fusion360 with either a saved database of cabinets or using a lot of custom parameters etc.

We try to keep the very complex 3d stuff inside fusion360 and the more cabinet related parts inside the cabinet software. If you figure out how to make Fusion360 use the drill block let me know ;)

Aside from that and the occasional slow performance under very complex geometric shapes I find Fusion360 very easy to work with and the direct to CAM integration is quite nice. Toolpaths are adequate and I have not found any problems with the Code it posts. It simply works and gets the job done. We make a lot of one off higher end projects that require a good bit of 3D toolpathing. This so far has worked quite well for us. We also make CNC machined metal parts and 3D SLA print things for our customers using the same softwares.

Pete

Hi Peter.

Not Fusion but we had a similar issue with SheetCam a few years ago.

What we did was reserved a series of tool numbers for the drills, Our machine had those spec'd. Started at 101.

The we hard coded the offset of drill 101 to the spindle (X, Y and Z) in the post and then the offsets of the rest of the drills to 101. X32, X64 X96 Y32 etc.

From there it was easy, If T>100 use ...

Verify that the spindle is up and use the drill commands.

Voila.

Thanks Dropout, As I said I am quite sure it is possible to use this multi drill head inside Fusion360. Of course setting up tool offsets would work. I think the difficulty comes from the CAD side of things. I do not think there is a way to say select a series of 32mm holes spaced and have the system understand that it is to use the multi drill head all at once calling out the individual tools and using their particular offsets for the holes at hand. Does that make sense? Again from what I have seen of the capabilities of the software it would not surprise me if there was a way to do this but I have not had time to mess with it.

Sheetcam was the very first CAM program I ever used. Worked great for my little CNC mill I built. I know it was really designed for CNC routers but works fine for me. I don't use it anymore now have switched CAM programs several times since then.

Right now we are using Mozaik and it has built in support for the multi drill head and they even made us a post for it so we use it that way most of the time. Who knows what the future will bring and what software we will be using hehehe..

Pete

To your last note:

Yes, BWorks looks at the direction and distances and will synchronize bit use in the optimization process automatically.

I assume your tools are set to sync and you have done this in BW directly. If not, try it and if it works, generate a cix and compare the piece and macro variables with your 360 cix.
It should not matter if you have a single routine of a line of holes or any number of individual bores along x at 32mm spacing.
I'm not certain but I believe you have access to tweak the 360 post if you need.

On the disappearing geometry:
This usually happens when BW can't make sense of the geometry (curves without solution, etc.) or programming rules are being broken (lead in geometry behind start point, etc.).

OK.

It's been a few months since I posted this here as well as on the Autodesk Forums and it we have made progress!

Drill Block - as long as the name of the tool and tool holder match in Fusion 360 and Biesseworks, everything works fine. As long as the holes are correctly spaced, multi-hole drilling works great!

Broken Geometry - this was the tough one. The most common reason for broken geometry in Biesseworks is when toolpaths cross outside of the working field. This doesn't always happen, but sometimes when a linking move, etc. goes outside the working box, Biesseworks thinks the line is broken. Easy fix has been to just nudge those parts further into the sheet. This means a bit more material waste, but this is better than no cuts at all!

Here's hoping the Fusion 360 team keeps improving things (and thanks for finally integrating nesting!)

Hi there

I have recently perfected a post processor for a Biesse Klever machine that outputs clear code when opened in BiesseWorks. It also allows for tool radius compensation and resolves the issues caused when implementing this.

If this would be useful to you, or you would like more improvements on your post processor, please contact me at michael@thepostmaster.co.za. I will be happy to provide you with this service.

Michael