2D Pocket toolpath having issues after updates

[kellyCL9A8]

Is anyone else having trouble with 2D Pocketing not generating toolpaths for the same pockets since the latest updates?

I use 2Dpocket to engrave my company logo into all of the parts we manufacture, I use this same logo and engraving on 40-50 different parts and we have run thousands of parts using this same toolpath. 

I am trying to run some parts from a fusion design I have been running about once a month all year, I had to change a tool number as I already had the tool loaded from the previous job (I do this all the time, so it's not uncommon to change this particular program),  but as soon as I generate the toolpath again it does not toolpath one pocket. I have tried to re-program that one pocket only with no luck. I was using a .dxf as the geometry, so it cut the logo into the part and then used the pocket as the pocket selection. But all I can get from it would be best described as a facing pocket that must be using the stock shape as its driver. 

As I have already said I have a lot of parts with the same logo that are already programmed and running, so I am hoping this is a bug from an update that can be fixed, as I am not really looking for a workaround.

I have been using Fusion 360 as my sole CAD and Cam package since 2018 so I do know my way around it fairly well and have tried all the tricks etc that I have found over the years, I will find a workaround to get the job completed but it would be great if 2d pocket can function as well as it has in the past.

Cheers

[HughesTooling · Accepted solution]

The problem seems to be the tolerance, if I set it to 0.01mm it seems to work. Are your old toolpath that work using 0.1mm for the tolerance?

Mark

[kellyCL9A8]

Hi Mark, yes all the toolpaths are the same 0.1 and for whatever reason (I know there has been a lot of work going on with 2d pocketing over the last couple of updates) generating the toolpaths for this program again even with zero changes it now can find a solution for the c pocket.

I have tried changing the tolerance, and you are right it does work like that, I know when I originally programmed this smaller logo back in early 2020 if I used a fine tolerance the toolpath had so many points in it that it would not run smoothly hence the 0.1 tolerance, which was about the best compromise I could find at the time. I have noticed over the last 6 months or maybe more that fusion has been much better at keeping the points to a minimum without any tolerance intervention which is nice.

Thanks for the help, if all I have to do is change the tolerance to get all the programs to run again then it is not to big of a deal. It also looks like the new toolpath will give me smoother looking curves to the logo, which will be a little bonus. 

I had worked around this by cutting the logo pockets into the model and used the 3d Horizontal toolpath which worked fine, I just tried it now and it will cut the c pocket with no problem with a 0.1 tolerance, but it does have a lot more points in the toolpath, go figure. 

Thanks again for the help

[Dave.Sohlstrom]

New user to Fusion 360 CAM The problem that I an encountering is I have a 5mm wide pocket 5mm long center to center that no matter what I have tried so far using a 3mm end mill sim shows the pocket being machined far bigger that the model.

Thanks for any help

Dave

[kellyCL9A8]

Hi Dave,

If you can export the file and attach it to a post in this thread someone might be able to help you out.

Cheers Kelly

[Dave.Sohlstrom]

OK here goes nothing. first try at attaching a file.

The problem is the last 2D pocket op.

Dave

[Dave.Sohlstrom]

Well wouldn't you know. after posting my file I was looking for more info and the answer to my problem was 3d pocketing. Got it running fairly well. does spend some time cutting air feeding down to the model surface. Then cuts the pocket in 2 passes. I can live with that. This is a one off so a little extra time cutting air is no big deal.

Dave

[kellyCL9A8]

Hi Dave,

Firstly I am not sure why you are modeling all in surfaces rather than a solid? I could be wrong, but from my experience, it is harder to model with surfaces and the model is not as easy to alter as you go, just things like you want to cut a hole into the side you also have to build the side wall and floor etc. If you need a surface then it is really easy to just create it from the model. 

Getting to the point, you are using the face as your pocket selection so it is machining all the way off the face to give a clean surface. I will try and attach your file modified which I have got the toolpath running. You need to select the edge of the pocket not the face to define the outer edge. Then the pocket is on the small side but if you reduce the minimum cutting radius down to 0.5mm or even 0.25mm then it will toolpath the pocket. the current 1 mm radius is to big to allow the tool into the small pocket.

I do a lot of this kind of machining on small pockets like this one and I would use 2d contour and then use the ramp lead-in function to get to the bottom, I also would mostly not leave stock as the small cutter will tend to push away from the wall a touch, and do a multiple finish pass of 0.025mm this acts as a spring pass, with only adding one pass at full depth (not another fully ramped in toolpath). It is good toolpath option when using a small cutter like this 3mm because it gives you effectively a helical type cut which is easy for the cutter to take without side loading and snapping off at your collet.

I find it works better than pocketing when the cutter you are using is the same or bigger than half of the pocket width, so does not need multiple passes to clean out all the material, it also gives good control of toolpaths in narrow pockets that are weird shapes.

I am sure there are lots of other opinions and ways that other members would attack this pocket, this is just my 2 cents on how I would go about it and what I did to get your toolpath to work.

Cheers Kelly

[Dave.Sohlstrom]

Kelly This part was modeled using Alibre. I have been using Alibre for years and can model there far easier than in fusion. the model was then exported from Alibre as an igs file and imported into fusion. I will down load your mod. if I have to I'll try and model the part in fusion.

I need to read your post several times to get a handle on what you are saying.

Thank you for your help 

Dave

[kellyCL9A8]

Got it, model it what whatever way works for you, it was just an observation. I have had issues with models like that not wanting to toolpath for me in the past, but in this case I think you are fine.

What I was describing (probably badly) I have got toolpaths in the file to show what I am talking about.

Cheers Kelly

[Dave.Sohlstrom]

I was able to open you DL. Thank you.

One more question if I could

Ease there a way to copy a setup from 1 part to another.

Dave

[kellyCL9A8]

Yes, that is simple just have both designs open, click on the setup you want, Ctrl C to copy, change to the other design click setups then Ctrl V to paste. All the toolpaths from that setup will be copied over, you can also copy just one toolpath from a setup. Just click on the toolpath you want Ctrl C to copy, change designs click on the setup you want the toolpath to be included in and Ctrl V to paste.

[HughesTooling]

---

@Dave.Sohlstrom wrote:

Kelly This part was modeled using Alibre. I have been using Alibre for years and can model there far easier than in fusion. the model was then exported from Alibre as an igs file and imported into fusion. I will down load your mod. if I have to I'll try and model the part in fusion.

I need to read your post several times to get a handle on what you are saying.

Thank you for your help 

Dave

---

You will be better off using STP files as they will come into Fusion as a body rather than a set of unstitched surfaces.

Mark