Internal Port Machining - 3D Contour / Blend tool paths

[mike]

Hey guys, first post on this forum.  I'd like to start by thanking everyone on here!  I have yet to need to post as the search function has always helped answer my questions, until now.   

Running this on a 5-axis.  Attached is an image as well as the f3d file.

Internal machining

I'm trying to machine the inside of this runner.  I have tried many different strategies.  3D Contour comes really close but doesn't actually follow the port.   I know it will machine within the given boundary as seen from the 'Tool Orientation'.   I have tried using the multi-axis option, which seems to just keep the tool away from the edges better, but does not get any further down around this bend. 

I found this thread:

https://forums.autodesk.com/t5/fusion-360-manufacture/multi-axis-blend-flow-internal-machining/m-p/9...

It suggested using the Blend strategy.   All looked great, I downloaded the attached file but was never able to get a tool path at all, just a red X.   It kept returning 'Internal Cam Kernel Error'.

I don't quite understand the 'drive curves' selections.  I also suspect the surface may be an issue, although I'm not very good in the Surface workspace.

Thanks in advance to anyone that may be able to offer some insight.

Mike

[DarthBane55]

I've done several manifolds in 5-axis, a bit similar to your part.  Be patient, be ready to create a lot of dummy models and surfaces.  You need to block as many areas as you can, by using dummy models that will have a wall where you don't want the tool to go.  The manifolds I did looked good, but it was not a quick program to make, and really, Fusion is not really made for this as of yet (any Powermill cycles coming in maybe in the future will allow simpler way to do this).  Also I had to lie a lot to the software, saying my shank was 0.001" diameter, in order to be able to access some hard to reach areas (with the real shank, it wouldn't do much work, stopping way too short of where it could actually go).  Now how do you make sure the shank will not crash when you run this on the machine (after telling Fusion that the shank is 0.001")?  Lucky for me, we have a gcode simulator, so I was able to make sure, but if you don't...  I would say this is extremely high risk (I would even say, don't do it!).

I don't have time to open your file at the moment, sorry about that, but when I saw the title, I thought I'd give some pointers.  

You need to position your tool axis very carefully, because even with 5-axis, it does not really like to mill undercut areas, so by moving the tool axis, and do a few operations with different tool axis, I ended up covering every where, but like I said, it's not really made for this stuff.  Doable, but be very patient, and don't be shy to create dummy models that will simplify the areas for Fusion.

Not sure this helps...  😥

EDIT: I'll try to open your file in a bit though, maybe your part doesn't have as many hard to reach areas and it might be not too bad.

[DarthBane55]

Ok, had a look at your file, this is doable for sure.  From what I see, you have access from both ends of the ports right?  You intend to machine it from both ends and meet in the middle, or has to be done all from 1 side?

[mike]

Yes, access from both sides of the port.   Attached is an updated model, I re-built the internal lofts.  Blend seems to work better, but leaves some odd missed spots no matter what I change it seems.  I know its beta so maybe thats why??

[DarthBane55 · Accepted solution]

Hi, sorry I was already almost done with the 1st model, so I just carried on.  See attached file.

It is not 100% final, I kept the stepdown coarse, and I don't know what tool you have etc.  But the big end actually gives pretty good access, if you have a reasonably long tool and skinny holder, you could do it all from that end.  But in the file I went from both ends.  If it was my part, I would go deeper from the big end, as it is not undercut and the path will be smoother on the machine (less drastic direction changes. It's actually pretty smooth from big end).

The flow toolpath takes a long time to generate, so I left it really coarse.

I did the cheat, putting the shank to 0.01"diameter, but you can see that the shank would not hit when you simulate it.  The reason for doing this, is that otherwise it will not go much in the undercut, I think it only goes as far as the ball meets the shank, from the operation's tool axis view point, so that is very small.  By making the shank as small as possible, it goes in undercut much deeper.

There are a couple of paths that didn't generate, maybe it's a matter of finding a right setting in there, not sure, but I have 2 paths that did generate. 

It seems to me that flow can do undercuts, at least a lot more than contour, so for that one I didn't use the cheated shank, but maybe it would work even better with the cheat.

You can play with the linking too, maybe better to have a lead-in/out on each pass to avoid the link on the wall, or not, you decide.

You'll see that I deleted the cross holes, and 1 port, to make it simple for Fusion.  I would then copy the model and delete the other port when doing the 2nd one.

I hope this helps and can move your forward with the job!

EDIT: I just realized that the flow path is not climb milling...  just change that if you use it!  (You'd have many things to tweak anyways, but I just noticed this now...).

EDIT 2: You'll see that I created a copy of the model, and offset the port inwards a bit, for simulation purposes (set as the stock in the setup).

[mike]

Thanks a bunch!   I didnt even think of using flow for an internal surface.  AND, the lollipop tool definitely would work better here, I've been using a straight flute.  I should really get a correct teardrop shaped form tool I would think.