Order by island not working??

[WhiteRoomSkis]

I am setting up a bunch of nested parts that need to be cut out of MDF. I want to cut each part individually before moving to the next to decrease the machining time due to excessively jogging around raw table. I have used this function many times before without issue. But tonight after updating F360 to the 4/17/18 update and then setting up my parts, the order by island command seems to be not working. I'll share the file and generate a screen cast in a bit but I wanted to get this up in case anyone else is seeing the same thing.

 I have even deleted the 2d contour tool path and tried setting it up from scratch thinking I did something wrong but it still ends up with the same result.

If you have any idea please on what I'm doing wrong or if maybe the update made this a bit buggy let me know.

you can play with the file if you want FILE

Thank you!

[Lambodesigns]

Thanks...... but the problem is I have to cut at multiple depths and use tabs.  Some of the parts I cut are pretty small (around 1" square) and the vacuum table won't hold without some small tabs.  The other problem without using tabs is even if they cut OK the dust collection will suck them up off the table and then I have to fish them out of the dust bin.  

Just seems like this is something that should be fixed so we don't have to do any work arounds.   When it is really irritating is when I have an old file that I have to make a small change to and then I have to figure out a way to make it work like it did a couple of years ago because it goes from an efficient tool path to some random thing that takes a lot longer to run.  

[engineguy]

@Lambodesigns 

The system I showed is very easy to do and uses "Tabs" so you should have no problem there, to be honest I have never seen it work with multiple depths, this thread goes way back to 2018, it didn`t work then ??

Do you have a sample file from way back that worked with multiple depths that you can share ??

Stay Safe

Regards

Rob

[Anonymous]

For the record I have been using Fusion on and off for nearly 3 years as a hobbyist. I built a CNC machine in a friends garage and play around with it when I have time. The company I  just started working for uses Solidworks, yes the Solidworks CAM 2019 plugin by CAMworks. 

I was considering getting a subscription to have access to the G0 (rapids) commands that you guys took away for hobyists ...(Don't get me started) when I remembered to check this issue. 

Anyway, I do remember a time when it worked and a couple of weeks later it stopped working. Thank you to the others who posted a file as an example. 

In a previous reply it was suggested to open a thread in the idea station, I just wanted to know if it had been done and how I go about putting in my vote to make an upgrade. 

Thank you, 

[Lambodesigns]

I've attached a file that shows the problem.  It is for displays I make and I've made over 1000 of them.  Originally, I was using sheetcam and a combination of CorelDraw and Sketchup for designs.  I converted it over to fusion a few years ago and cut several hundred with no problem.  Then..... a workaround was needed because I made a small change to the file and regenerated the toolpaths.  Needless to say, several hours were wasted since this used to work and then all of a sudden it didn't so it took a while to find that fusion had changed so what had worked now doesn't. 

The parts are sitting on top of my vacuum table that uses a series of holes that are on 1" centers.  I use a fixture on top of that that eliminates the through holes where the bit cuts through so the vacuum isn't lost as the holes are exposed.  Since this had worked great for so long I really didn't want to build a new fixture to get around this issue so moving the parts around is not a good option.  There is a setup with the work arounds and a setup that was how I originally cut the parts so you can see the difference in the toolpaths.  There is also a toolpath based on a pattern for the wedges that cuts the parts out in an "order by island" fashion so it is still possible to get around the error by using that method as long as the parts are all the same and on a grid.  There is also an example of the tool paths for the cutouts that the wedges go in using "preserve order" where you can see that the order is not preserved and the bit is going around in a random order.  As I said earlier, I've made over a thousand of these so the time to cut is important and watching the router rapid all over the place is not an option.  Bottom line is these functions used to work and for the last couple of year they have been broken.  

[engineguy]

@Lambodesigns 

Not able to open your files, lots of files zipped up that have external references so won`t open here 🙂 🙂

Stay Safe

Regards

Rob

[Lambodesigns]

It was only giving me the option to export as a f3z file.  I guess when there are linked parts it won't export as an f3d file type.  Had to go in and break all the links and it then allowed me to export as a f3d.   Quick check and it seems to operate the same way with the tool paths.   Hopefully, this will work.  

[Anonymous]

I was hopeful after reading your post last week. However the trace doesn't do two things I like to use. 

1. You can only specify a lead in and lead out, I like to ramp into the material. 

2. Specify the entry point. I use this to prevent the part from breaking away on the final cutout as it reaches back around. I ensure the tool enters and finishes where the material is not touching some previously milled material. 

Best

James

[gumballelectronics]

Yeah this has been totally frustrating me trying to learn CAM. Disappointing to learn it's been going on for years without a fix. Guess I'll have to keep doing multiple paths manually.

[trvs.king]

I agree with many above. All Autodesk employees just responding that it's by design, when not answering for what the rationale is are coming across as obtuse. Here I am tediously creating individual contours so that my parts fall out of a maslow nicely when I could be spending time on something substantial. Just get rid of the feature if all your customers hate it. Autodesk, not Manually-Click-Duplicate-Desk

[to3dornottobe]

It can't think of a reason why this 'meant to be' feature is better than what we're asking here.

I gave it some time to let it sink in and thought about it for a while, but i'm unable to think of a situation where this design feature is practical in this 2d contour application. I'd like to know why it is designed the way it is. Perhaps it can be benificial for some of us as well. When nesting parts for a vacuum workholding it's an annoyance for a long time.

Nested parts, 18 pcs: what I do to overcome this flaw is duplicate the toolpath 18 times.. So by design I need to duplicate the toolpath for as many times as I want to use the features description. That is inconvenient. 

[Lambodesigns]

The worst for me is when I have an old file that worked the way it should and then I have to make a change to a part. Then when I regenerate the g code I'm forced to go in and spend a lot of time to make it operate like it did because I changed something minor within a part like moving a hole a small amount.  Extremely frustrating especially considering how long this has been broken and fusion doesn't understand why it should work the way it used to work..... 

[engineguy]

@Lambodesigns 

@WhiteRoomSkis 

Have either of you tried using the Trace workaround, it will do what you want, just have to watch the Leadin/Leadout values, just a different way to do it,  If you make a change in Design then in Manufacture you only need to Re-generate to get the new toolpath, actually not any harder than using the Contour toolpath, just different 🙂 🙂

Try the attached file and change a shape or two and the toolpath will re-generate no problem 🙂

[to3dornottobe]

Thanks for your effort. Although I abuse the trace function for 'chamfering' with a ball endmill,  the ramp feature is missing for this specific goal. And it also lacks the advanced lead in/lead out, not giving me the option to do an angular lead in. When cutting 25-40mm thick MDF/plywood you need to ramp into the material instead of the normal lead in/out. And with melamine chipboard I like to use an angle at the lead in, to avoid breakout of the melamine at the bottom. 

Both of these functions are missing. So, no. I can not use the trace feature making the same quality cuts as with the features offered in the 2d contour.

Can you give a technical motivation why this less appreciated feature we are forced to use is implemented in the 2d contour nowadays?

[craptree4NU47]

Hi, sorry I know this is a long running thread, but thought I'd post here as I ran into the exact same issue  - extremely frustrating!

I managed to work out quite a good solution though that doesn't need the use of any alternative tool paths.

If you run the 2d contour toolpath with multiple depths disabled(under the Passes tab) the islands feature works. If you need to use multiple depths, you can use the better option of running the depths as part of the Ramp feature under the Linking tab. Use the "Maximum ramp stepdown" to set your cutting depth on each path.

This works perfectly for me - islands are cut fully, 1 at a time, you can use the tab feature of the 2d contour toolpath, and you can still cut via multiple depths.

Any issues let me know

Riz

[to3dornottobe]

For some occasions this if fine. With HPL coverend birch or melamine covered chipwood, you can't use ramp. If you use ramp, you'll damage the downfacing layer sooner or later. You'll need a relative low angle lead in to avoid the tool from protruding right at the edge of your workpiece. (you normally cut at -.1 or -.2 mm in the spoilboard in my line of work. 

[craptree4NU47]

Yikes yea I didn't consider MFC, that would definitely be a problem, we
only use solid wood at our company so haven't experienced that yet. Good to
know though if we get any projects that use it.

[infoH2EV4]

Hi,

that works, thank you!

But I can't use ramps then. Thats a pity. 

I always need to duplicate the operation and selecht each contour separately.

Autodesk, would you please add an additional feature sort by island that works in the desired way?

regards

rainer

[to3dornottobe]

Yes Autodesk. Please make this function work again. It doesn't make sense at all the crippled, flawed and buggy way it limps around now. Just kill the flawed feature or make it work again.. 

[engineguy]

@to3dornottobe 

Daft thing is that it does work OK as long as the items being machined are more than double the diameter of the tool apart, why they have this in is a mystery to me !!! Please Autodesk, please remove this silly limitation as quickly as possible, it means a lot of wasted material that costs $$$$$$ !!!

[seth.madore]

This conversation has come up multiple times over the years, and the last time it did, the verdict was "working as intended, no plans to change". I can always poke them again and hope I catch em on a good day...