Fusion360 Turning Rough Profile Pecking is sloooooow
@Eric_Evans_a_GiroDisc_com wrote:
2 Questions
1-Why are the peck retracts posted at the cutting feed rate? These should use a lead out feed or rapid.
That's a good question, I'll check with the developers to see if there are some limitations we're working under. Would you expect to see a lead-out feedrate, but a cutting feed to return, or do you expect lead-out and in and then resume cutting feedrate?
@Eric_Evans_a_GiroDisc_com wrote:
2-Why can't you only feed in Z? Roughing front to back I just want to go straight in Z, I don't want to drag the tool up in X at the end of the cut. Enabling "No Dragging" just flip-flops the cutting direction so it pushes from the outside in, as opposed to dragging inside to out in X.
Can you expand more on this? You want to only go in Z and then rapid back in Z with the tool still contacting the part? Or am I misunderstanding what you're asking (I think I am)
For item #3, can you share a file that shows this wasted move and what you want to be able to adjust to improve your cycle time?
Seth Madore
Customer Advocacy Manager - Manufacturing
1-I would expect the turning pecking to be handled just like selecting a drill cycle, rapid out is an option, but so is feed out. If we were provided with fill-in-the-blank retract and return options that could be sweet but I'm not sure that detailed level of control is necessary.
On that note I do think all roughing cycles could benefit from the lead-in and lead-out feed parameters.
2-All passes overlap in roughing so it cleans up ALL the stock. Similar to pecking, I just want the tool to go forward, then back. Or at least have control over how much the tool "lifts" before retracting:
That circled wedge shaped chip is going to come off the part as a big curly ribbon, after doing that all day long my chip conveyor is going to be jammed up.
If I use no dragging it breaks each move up into a pair of Z and X moves, this could just be a bunch of Z moves and then one X move.
I would also be fine if it left that cusp at each stepover and I could come back in a totally separate operation to clean it up.
3-This:
Why does the tool go all the way to the extent of the cut, then traverse back to the start. It also does this but in reverse for OD tools. I would prefer if the operation started at the top, where the cutting actually starts...
If your part is 11" diameter that's a lot of miles going back-and-forth from OD to centerline (or feature ID as shown)
I would like to see something like this but for X:
I've been troubleshooting an issue for a while now and am thinking this roughing overlap may be contributing to my woes.
We make frisbee shape/size parts and flatness/parallelism between the circled faces is very important to the function of the part; we require under 0.0010"
I have programs for this part generated in Fusion and MasterCAM using the same cutting parameters; same SFM, same max rpm, same IPR, same stepover, same stock for finishing, etc...
The MasterCAM program makes a part flat/parallel within 0.0003", while the Fusion part is hovering just around .0010"
After chasing my tail for a while double checking cutting parameters I started looking at the actual code and noticed the roughing in Fusion "overlaps" to the exact same value as the previous pass:
While the MasterCAM code overlaps to the same value, and then extends an additional 0.0200"
If I had any sort of discrepancy between my programmed and actual tool radius this could leave a cusp, and during finishing may result in a wavy surface. I do not want to run a spring pass because finishing must be run incredibly slow to achieve the desired RA.
I could add a semi-finish to smooth out these cusps but that seems like a waste since it already comes so close to smoothing out the surface... It would be nice if you could just control this overlap value instead. In some instances it might be nice to run with zero overlap (straight in/straight out) and follow up with a semi-finish path to smooth it all out, and in others you may way to increase the overlap to ensure there is no cusp left and call it done in one.
Any ideas on how to solve this without having a bunch of extra motions/operations?
How does MasterCAM calculate this overshoot from the prior pass? Tool radius plus fudge amount?
Seth Madore
Customer Advocacy Manager - Manufacturing
@Eric_Evans_a_GiroDisc_com wrote:
I would also be fine if it left that cusp at each stepover and I could come back in a totally separate operation to clean it up.
In post #3, you made this statement above. Doesn't that contradict your most recent observations?
(Mind you, I'm not so much challenging your thoughts/explanation, but trying to drive clarity to how we can better improve this product so it provides you with the turning solution you need for your applications)
Seth Madore
Customer Advocacy Manager - Manufacturing
You can control the amount of overlap. You can also straight-up disable it.
While I've got your attention multiple depths in rough turning would be a nice feature to add.
I have very few significant grips about CAD and Mill CAM in Fusion, but man... lathe CAM just lags so far behind.
Everything in one platform, and all parametrically linked is awesome. Recognizing geometry and updating toolpaths is soooo sweet. I can program and confidently be running a prototype part for our dual spindles in <8 minutes thanks to my templatized workflow in Fusion vs. 20+ minutes in MasterCAM.
But if it can't make parts in spec then none of that matters...
Variable depths for roughing? It's been a while since I've used Esprit, but I don't recall that software offering that flexibility 🤔
And yeah, preaching to the choir here; I use Fusion to run my shop and it's been a long time overdue where the gap between Mill and Turn needed to be closed. The nice thing is (as I have an inside view to development) and I'm just gonna say; we have some really nice improvements in the pipeline which the Commercial user is going to see before long.... 🤐
Seth Madore
Customer Advocacy Manager - Manufacturing
So then, if I understand, you'd like to see a toggle to change whether or not you want any overlap at all, and also define additional overlap as the job requires, is that correct? (I think it's a great idea, fwiw, just trying to make sure I capture your needs)
Seth Madore
Customer Advocacy Manager - Manufacturing
We've added all those thoughts to existing (and new) tasks. Obviously, I can't make any promises as to "when", but they do line up with our goal of producing better value for the shops who focus on Turning efficiency.
Seth Madore
Customer Advocacy Manager - Manufacturing
@Eric_Evans_a_GiroDisc_com (2) was added in the update that recently went out.
Regards,
Akash Kamoolkar
Software Development Manager
