Using boring bar for both ID and ID

[whamilton121993]

Hi All, 

I am trying to use a boring bar with a threading insert to profile both the ID and OD in one operation to cut out a ring, i have created a custom grooving tool with a very thin tip to model the point on the threading tool

I am trying to profile both the OD and ID without a tool change. I am able to do one of the operations without an issue - here is the ID profiling

This works well however the issue comes when i want to cut the outer diameter

I have tried creating a duplicate of the original tool and tried to change to orientation/ spindle speed but this has not worked.

I am wondering if anyone has any tips on how this can work?

Thanks,

William

[Anonymous]

You need two toolpaths with same tool but different value in "turret" field of post processing tab in tool definition, one for internal work where turret number in is 0 (zero), and second one where turret is set to 101.

You also need to assign different offset number to second toolpath so you can control sizes independently.

Post using Fanuc generic turning post from HSM library, basically setting 101 in second tool path will be mirrored about Z axis, all X values will have negative sign in front and CW/CCW arcs will be inverted.

[Anonymous]

Just one inconvenience, this is not part of normal activity so you will probably come up with tool incompatibility when you try to use boring bar below center line. What you do is program two paths separately,  use left hand turning tool inverted and running with M4, produce code for OD then post with that 101 setting, combine programs and use boring bar at the machine. 

[Anonymous · Accepted solution]

Here it is, I mislead you on tool orientation for turning so I had to find out what works.

You need to define separate tools because of orientation, after posting make it same tool and assign different offset to second operation so you can control sizes independently.

[whamilton121993]

thank you, i'll give this a go.

What is that g-code viewer?

[whamilton121993]

Hi @Anonymous,

I have had a look through your solution and the G-Code works perfectly, it's exactly what i'm looking for.

However i'm still a bit confused as to how you managed to get it to cut like that, here is the simulation below, but the g-code seems to produce the correct profile, how did you do this?

Thanks,
William 

[Anonymous]

I am a magician, that's what I do 😁 ,.... but seriously, if you look at tool definitions, boring bar needs no explanation but using boring bar as turning tool does.

So basically you are programming turning on positive side of X axis, keeping in mind fixed position of boring bar, you define tool for orientation equivalent of that when you position boring bar to cut OD on negative side of X axis.

For fixed orientation of boring bar to cut OD, you have to reverse spindle direction.

Simulation shows boring bar cutting OD on positive side of X axis but post processor setting of 101 in turret field triggers negative X axis output and reversed arcs.

Spindle rotation must be towards cutting edge depending on tool orientation and arcs are always in reference to clock and start / end point of arc move.

Confusing factor may be that bar is cutting on opposite side of center line, but it's really the same because you are rotating boring bar about Z axis and cutting on negative side of X axis, the magic of correct NC code output is done by post processor, and not just any post processor, that's why I included it in zip folder to save you the trouble of downloading it from HSM library. 

Due to different spindle direction in two operations, you have to define two separate tools using same physical tool, 

after producing code, just edit tool to be same number but different offset.

[whamilton121993]

Perfect, thank you! sounds like a bit of a bug in the simulation code to display it on the wrong side?

[Anonymous]

I wouldn't call it a bug, just the fact that Fusion locks refinement and full development of some feature but still allows you to produce desired results,..... if you are magician. 😋 

[whamilton121993]

Hi @Anonymous ,

if you have a spare few moments would you please be able to tell me why the attached file is not working as the f3d solution file you attached is?

Thanks,

William

[whamilton121993]

Nevermind the turret number sorted it! Thank you!

[Anonymous]

The initial file I showed you is applicable concept, however, there are some complications when you try to do awkward things. I took interest in your file just for kicks and ended up with numerous issues that don't seem to have solution.

You have not defined tool completely, you have to define every field for tool to take shape in graphical window.

Once you do that there are other problems, model dimensions are such where if one tool runs, the other will separate the ring from stock before completing full tool path because it overlaps with cut profile from other tool.

I gave tools .2 mm corner radius, in single point turning, tool has to have some value of corner radius or it will leave stairs on finished surface.

While running OD profile, I cannot force tool to leave same amount of stock as in ID profile, it always leaves a lot more.

I tried using sketch as geometry selection, shifting inner height, nothing works.

If I set to not allowing undercutting, it still does undercutting.

There is something wrong with using grooving tool as turning tool and I have no fix  for that, it's a bug.

Considering geometry of your model, I would suggest using conventional tools with operations that work as expected, you can still post tool for OD profile with negative X axis orientation and change tools as needed.

Below is file with some progress and issues I mentioned, no need to try impossible unless I missed something.