Radius issues, file.

[kretallick144]

Complete file from fusion.

[Anonymous]

I reset few things in file, after posting for positive X axis lathe using Fanuc generic post from library, I mirrored X axis and swapped G02 / G03 using NC editor found at this link https://www.cnc-syntax-editor.com/

[daniel_lyall]

And the problem is??????????

[Anonymous]

Free backploting software

[Anonymous]

Ideally, have post edited to output negative X axis and swap G02/G03, but if not, few steps I showed you will the job.

I would use I and K instead of R, in which case I would have to be mirrored as well.

I overlooked one thing, never use constant surface speed in threading, always use strait RPM.

In this case G97 S500 may be good start and you need to make more then 6 passes to avoid chatter because of thread being so far out from spindle.

It may be a good idea to only turn front end, thread it then turn the rest of the shaft, that way you use stock to provide more rigidity for threading.

[kretallick144]

Thanks.

Im using dnc4u to edit the code.  Comparing the 2 i cannot see any difference in the lines with R.

These are the outside radius on the step up to larger diameters.

I do plan on changing the threading to be done before the rest of the machining. ATM everything is working except these **** OD radi.

[daniel_lyall]

@kretallick144  it is quite posable that it is a bug the 4 picks below are 3 diffrent tools and 2 diffrent models the first 3 are from doing a revole and last one is what you did the out come for the tools are very much the same with each version.

I am not a %100 certin that is a bug but 4 set of eyes will not hurt and also I think there is bit of a graphics error in the sim.

@seth.madore Can you plese have a look 

Tool 4

Tool 10 

These two use this shape tool

[kretallick144]

My simulation in Fusion shows its following the toolpath fine.

Is there a way to show line numbers during simulation?

Cnc syntax editor looks very similar to dnc4u, My trial for dnc4u is about up, Is there a preferred software to purchase?

[Anonymous]

---

@kretallick144 wrote:

Thanks.

Im using dnc4u to edit the code.  Comparing the 2 i cannot see any difference in the lines with R.

These are the outside radius on the step up to larger diameters.

I do plan on changing the threading to be done before the rest of the machining. ATM everything is working except these **** OD radi.

---

DNC4U or syntax editor, it doesn't matter, use whatever, they are just tools to mirror the NC code.

If post produced good numbers and you mirrored X axis it should work, if not try different post, use I and K instead of R.

Is there a problem with model?, I'll have a closer look later.

[Anonymous]

You had tool set to "tip" instead of "tip tangent".

If you are starving artist and your CNC4U trial expires, software I pointed out is FREE, never expires.

Here is corrected file with updated NC file.

[Anonymous]

Here is identical file using I and K

[Anonymous]

Well after some more snooping around I see that there is a bug in Fusion turning profile where two fillets are tangent to each other.

I separated roughing from finishing and ran simulation, it goes thru as expected but when posted using two different posts, result is the same, both have bug.

I then programmed finish pass in Mastercan and all is well in the kingdom.

I will update your roughing NC file later, for now here are the screen shots of what's going on.

Fusion 

Mastercam

[Anonymous]

Here is your updated turning program correcting bug resulting from Fusion post.

Disregard tool orientation, tip is all that matters here and it is in sink with part profile.

[Anonymous]

Ops............... mixed up units,  file is in inch unit and I corrected feed rate.

[daniel_lyall]

@Anonymous well-done learned something new today.

[Anonymous]

Heck, I thought wrong tool tip was the only issue at first but there seems to be a real BUG here. I haven't encountered it before since much of my turning work is done in Mastercam and for times when I combine it with mill work I carefully back plot all turning because I don't yet trust Fusion turning 100 %.

[daniel_lyall]

There is definitely something not quite right with the tool path, changing to a small diamond shape tool the toolpath looks better.

This looks very wrong to me the yellow is the model's outline blue is the toolpath.

[akash.kamoolkar]

My two cents here, there doesn't seem to be anything wrong with the path of the tool. The reason the radius of the toolpath arc is much smaller than the radius of the arc of the fillet is because you are machining a concave arc with a tool with a comparatively large tool nose radius. Geometrically since the contact point of the tool keeps changing throughout the arc, the resultant toolpath arc is going to be much smaller. You can verify this by simulating at a very slow speed, turning on the program point option in the simulation dialog. You will see the tool never gouges, remains in contact with the model and the program point follows the tool faithfully along the toolpath.

Another way to test my theory is by making the tool nose radius smaller. As it gets smaller, the radius of the toolpath arc will approach the radius of the fillet.

There is another issue with the toolpath though and that is the fact that the NC code to machine the first radius is getting broken into lines and I will create a ticket for that.

Regards,

Akash Kamoolkar

[daniel_lyall]

The small tool shows that the toolpath improves with what victor said above it makes it look ok, it is just that the toolpath looks to be inside the model what I think it should not do.

The flat-looking bits on two of the radius in sim looks to just be a graphic error back plotting the Gcode proves this and what you think.

[akash.kamoolkar]

The program point (tool compensation point) is set to tip, which means it's the "imaginary" intersection of the two sides of the insert. That point will always be inside the part for that type of geometry, especially with a large tool nose radius. Look at the picture below

Akash