Adaptive Clearing Bug, i think...

[m_carreira3Y72Q]

I am relatively new to Fusion. Up until now i have been using adaptive clearings all the time for roughing operations, and i have a few issues with it, in fact i think it has some bugs.

i attached a file where i replicated some issues i have with real parts i am currently milling.

The attached file has 5 setups, they are all the same, except for one of the milling operations within each of them.

Each Setup has a folder called "Stock Simulation", i did that because i am currently milling some parts that are cast, to final dimension plus 0.2mm, and fusion does not have an option to consider that the starting point for a setup is the model plus a certain amount of material arround each wall. (That was a HINT... it would be a nice feature) So i start with a block and an adaptive clearing with an axial and radial offset of 0.2mm. I dont run that program in the mill, i just use it to update the stock to what it really is and i named that milling strategy "IgnoreThis".

The first setup is called Adaptive OrderByDepth, and if you highlight the Adaptive clearing operation you will see that it wount mill the whole part on the outside for some reason.

The second setup (Adaptive clearing normal Order) is a copy of the first, but in the Adaptive clearing operation i didnt check order by depth, and if you highlight the trajectory you will see that it will now mill the outside of the part.

I really think this is a bug.

The 3rd and 4th setups are respectively copies of the 1st and 2nd, but instead of milling the same part, i created a manufacturing model assigned it to both the 3rd and 4th setups and then i removed the hole in the midle of the part.

And just like that, the exterior of the part is now always completly milled, regardless of ordering by depth or not.

Another problem is the retract heights, i get warnings in all the adaptive clearing operations "lifting retract height to safe height" and "lifting clearance height to retract height", but there is no way for me to define the "safe height". I think all other operations or at the least most of them have that option, and the warning messages tell me that Adaptive Clearing has that parameter too, but for some reason it must be hard coded (or internally calculated, somehow) and not acessible to the user.

If you select the 3rd and 4th setup there is a little sketch with a ruler, that alows you to see how far the retracts are above the heights i selected for the retract and clearance planes.

The fifth setup is a another copy but instead of an adaptive clearing there is a pocket clearing operation, and that one seems to work with both models, no matter the order i chose, and despite a few warnings it actually respects the retract heights i chose.

I think Adaptive Clearings are bugged, but please correct me and point me in the right direction if i am wrong.

Thank's in advance.

Miguel Carreira

[programming2C78B]

"fusion does not have an option to consider that the starting point for a setup is the model plus a certain amount of material arround (sic) each wall"

you can create a sketch point on the location you want to use as your g54, or a stock model, etc.


"but there is no way for me to define the "safe height"
It's in your last tab on every other toolpath. All you need to do is raise your Retract height to be above your stock.

I appreciate that you added so much information. 

[dpm-lic01]

"you can create a sketch point on the location you want to use as your g54, or a stock model, etc"

Why? Unless i didnt make myself clear, i dont have any doubt about te WCS, by starting point, i mean the stock for a part, i can have a cylinder, or a block and a few other options, but it would be nice to create a setup and define the starting stock is the mudel plus some ammount of material around it, that is what i meant.

""but there is no way for me to define the "safe height"
It's in your last tab on every other toolpath. All you need to do is raise your Retract height to be above your stock."

It does not work in adaptive clearings, no matter what i do i cant have my retracts below 2 or 3 milimeters, and there is no way to modify that.

I would really like an explanation from a dev about these issues, like i said, e really believe they are bugs, especially the order by depth option having an effect on how mutch of the part is milled on the out side, and the fact that a hole in the center of a part, changes trajectories created with adaptive clearings on the outside of the part.

[dpm-lic01]

I replyed as if i created this post, because i did, with a different fusion accounts (m_carreira3Y72Q), sorry for the confusion this might cause.

[seth.madore]

---

@dpm-lic01 wrote:

It does not work in adaptive clearings, no matter what i do i cant have my retracts below 2 or 3 milimeters, and there is no way to modify that.

---

There is a "hidden" minimum retraction value of 2mm. I never noticed it myself, since I had my Clearance and Retract set to .100" above. But yeah, it's baked into the toolpath and there's no plans (to my knowledge) to change the behavior.

I'll look into your other comments and views today (hopefully). Poke me again if you don't hear back in a timely fashion! 🙂

[m_carreira3Y72Q]

That explains the retracts situation, i was trying to get it below that to reduce milling time, i am currently roughing parts with a 1mm endmill, that is why my stock for roughing is 0.03 and 0.05 for radial and axial.

And i work in series, every second counts when dealing with orders of hundreds of parts, so having a baked in 2mm clearance doesnt make mutch sense to me, when dealing with parts that in some cases are smaller that that along the Z axis.

Besides all that i think the adaptive clearing retracts way too often, and if the tool is above the part, it is not cutting.

Thx for your time.

(replying from my actual account now, the dpm-lic was the test account our software provider gave us to test, before purchasing fusion)

[seth.madore]

---

@m_carreira3Y72Q wrote:

I did that because I am currently milling some parts that are cast, to final dimension plus 0.2mm, and fusion does not have an option to consider that the starting point for a setup is the model plus a certain amount of material around each wall. (That was a HINT... it would be a nice feature) So I start with a block and an adaptive clearing with an axial and radial offset of 0.2mm. I don't run that program in the mill, I just use it to update the stock to what it really is and I named that milling strategy "IgnoreThis".

---

Actually, there is a way to create a Stock Model with the additional material you're looking for! We have a tool in the Design workspace called "Shell". Now normally, it's considered to be a way to make a solid part hollow, but it also works to add equal amounts of material all over a part:

 

[m_carreira3Y72Q]

  With complex geometry it doesnt work well, its a very good tip, i had never thought of using it like that, and i will give it a try in futute projects. In this case it wount work at all with sharp shell selected(after reading the error message i tryed anything from 0.05 to 1mm and nothing worked), but it creates part of it if i select round shell, and it might be usefull, i can try to fix or create the missing surfaces myself, or maybe i get lucky in future projects and the geometry wount be this complicated...

The only other thing that i had thought of to solve this and never actually did, is using the method i am currently using, milling the part on both sides without fixtures with axial offsets, simulate, and then export the simulation result solid and use it as stock, but it would be even more work, on top of what i am already doing so i never tryed it.

The dialog boxes were left intentionally there to hide the part.

[programming2C78B]

You could also copy the model and scale it in all 3 dims so it's Xmm larger on all surfaces. 

[m_carreira3Y72Q]

Doesn't work, some exterior surfaces might give the ilusion that it will, but a cavity in the center of the part would just become larger, scaling just doesn't work like that, i can think of a number of reasons why, too mutch to describe here. If you want to see for yourself draw or download some complex parts and try it, it will apear to work on a cube or a cylinder with no other features.

[programming2C78B]

yes thats true. I only meant in regards to you being able to set your WCS a certain distance off the wall since you don't want to do a sketch point.

[Fabbunny69]

I don't have a model as complex as yours but using a window selection(checking everything is selected) to select my bottle and then 'Offset Face' 2mm did seem to give me a constant additional material offset for my stock.

Retract height; I don't think it's as important as the 'Lift Height', 'Lead & Transitions' & 'Ramp' in its effect on cycle time. I believe it is the position the tool will move to when the machining cycle is repositioning ready for the next sweep of cuts if there is an obstacle in the way, and it will be done either at rapid or high feed. I think it's important to ensure that the sum of your 'Lift Height', 'Leads & Transitions', and 'Ramp' is very close to the depth of the material being removed.

[m_carreira3Y72Q]

Whats that with the sketch point? You sugested that talking about G54, i dont have issues with my WCS, i dont know why you are sugesting that. My WCS is where it is, the center of the part. THe only thing that matters is that i center the part in the machine acording to where it is in CAM, we are not on the same page here. Please explain what you mean.

[m_carreira3Y72Q]

The surface offset doesnt work, the same happens with the shell operation. In simple geometry its fine with complex geometry it's not.

i had already tryed the offset faces before this post and it didnt work, the shell operation had never ocurred to me.

As for what i am calling retracts, the warnings i get are for both lifts and retracts, they are both too high. Like i said, in some cases a 2mm lift height is more than the height of the part i am milling. The one giving me trouble now is 3.9mm height for the finished part, so i have lifts that are at least 50% of the part height (imagine that with big parts, and your machines hitting its axis limits), also the adaptive clearing lifts way too often in my opinion.

The solution for me is avoid Adaptive Clearings for now, but the lifts and retracts are not the only issue, there are also thouse other problems i described:

The strange things that happen in some cases when you select order by depth, and how the part having a hole in its center affects the adaptive clearing's ability to mill the outside of the part, when order by depth is selected.

The part i shared in my first post is not real, i created it just to demonstrate the behaviour of Adaptive Clearings with simple geometry, but i had those issues in real parts i was milling, and that is actually more concerning to me than having a way to make my stock be the part plus 0.2mm, or whatever value i chose. That was only a suggestion, of something that would make my life easyer, but like i said i already have a work around for it, and i only mentioned it because i had to, to let you know why those programs where there in the example part i posted.

About the liftts and retracts, i already have my answer, as i suspected there is a hardcoded value for that, and the operator can't change it.