Help With Toolpath Verification

[oldtbone55]

@LibertyMachine

Hello Seth, 

I'm asking for your help with the CAM operations for a guitar neck that I've just finished modeling as you've been such a great help to me before. I've created the toolpaths but need someone to give them a quick review to see if there's anything wonky or if I could improve any of the toolpath operations. It looks like there's no way to create tabs for a 3D contour like there is for a 2D contour so I only have tabs on one end of the neck. Do I have to create tabs as part of the model for the headstock to get around this problem or is there another way? I've attached my file.

Your help is greatly appreciated. Thanks.

[oldtbone55]

@daniel_lyall

Hello Daniel,

I've run into an issue with my model. I can't combine my mesh body from Setup 1 (op2 stock) with the jig stock in order to create the shape of the jig for the CAM operations. I noticed in your file that your op2 stock is a solid body, not a mesh body. I did some searching on the forum and found some information about converting a mesh body (stl) to a solid but it isn't working. What I've found is that since the faces of the mesh body are triangular instead of quad, the mesh body may not be acceptable to combine with other bodies. Creating a base feature was another suggestion I found but when I tried that my file locked up and I can't move the timeline marker to go back so I can try and perform a merge of the faces. I can't turn the timeline history back on either and all of the bodies I had are now gone. Can you have a look at my file?

Thanks.

[oldtbone55]

@daniel_lyall

Hello Daniel,

I figured out the base feature (finish base feature) and then was able to roll back the history marker. I can convert the mesh body to a brep but I get a warning that it will slow things down dramatically because of the number of faces, plus I can't combine the mesh body with the jig stock to get the pattern I need to cut out the jig. Your suggestions would be appreciated.

Thanks.

[daniel_lyall]

I cant video the process my computers not powerful enough.

The steps are stay in base feature, goto the patch workspaces, select modify - mesh - mesh to Brep 

then

Create - boundary fill then, select tools is the model and select cells is the same thing

Then when that is done go back to the model work spaces and now the combine cut should work fine.

[oldtbone55]

@daniel_lyall

Hello Daniel and thanks for the info. I did what you suggested and was able to turn the mesh body into a solid body but still could not combine the two bodies as I got an error message (screenshot attached). I did get a warning when I was converting the mesh to a b-rep about the conversion having too many facets. Supposedly you're supposed to be able to merge the faces of the mesh body before doing the conversion but I couldn't get it to work. I'll keep researching this on the forum but in the meantime if you have any suggestions please let me know.

Thanks.

[daniel_lyall]

I was getting that as well that's why I was useing the boundary fill, but you have to make sure you turn the correct body off the original mesh to brep body fails with the combine the boundary fill body is fine. 

[oldtbone55]

@daniel_lyall

Hello Daniel, hope you're having a good weekend there. I was finally able to complete  turning the mesh body into a brep. It was a really intensive transition even with my laptop. I actually wound up with two of the Setup 1 stock bodies, one when I first converted the mesh to a solid, and a second when I used the boundary fill. I deleted the first body and kept the one after doing the boundary fill. I had no problem then combining the jig stock with the Setup 1 body/jig and got the jig body. Just as a note, I don't know if you are aware of the new mesh commands that are available after you've created a mesh body or imported an stl or obj file. It's a preview that's available by going into your preferences>mesh>click on mesh preview. I had tried to use this feature but it didn't seem to help my situation. There really is some heavy computing time with my model even with the gen7 intel chipset. I think I may need more ram. Anyway, I've attached my file for your approval and if everything is ok I'll start working on the CNC stuff this week. Do you guys celebrate Thanksgiving? It's the Canadian thanksgiving weekend (long weekend). 

Happy Turkey Day!

[daniel_lyall]

We have our own version of thanksgiving called Waitangi Day.

I know about the new mesh stuff It wont help with what you need to do so I said nothing about it, for it to be useful in cam they need to fix the conversion so it can have a minimum of half a million face's not 10000.

[oldtbone55]

@daniel_lyall

Happy Waitangi Day! Is a turkey part of the celebration or is that just a North American thing? Anyway, I agree with you, 10,000 faces is not anywhere near enough. I'm amazed that the conversion even works. What is the point of having these features if they are going to be that limiting when designing a model.  Let me know if my model is good enough for the next step.

Cheers!

[daniel_lyall]

I had to do changes to the contour on setup 1 it was cutting into the model I just used a - tangential extension distances to fix it.

The adaptives I just moved the tolerances on some of them back by 1 zero to stop some of the little cut nothing move's.

The second to last contour wont do a very good job of cutting nicely in the area where the arrow is pointing.

 

Other than that I think it's fine.

The stuff with the mesh not working very well and the stuff around that, I don't know why they have it like that they get baged for it every week, I wish they would fix it. I think it's down to them up the chain changing how they think fusion should be going from a very much a maker program to a regular cad/cam program, I think this is wrong but it will all get fixed up in the next few years.

Fusion will end up as a do all program within the next 5 to 10 years.

[oldtbone55]

@daniel_lyall

Thanks kindly Daniel for having a look at my file. I'm not sure why I couldn't replicate your toolpaths but it probably has something to do with me not understanding what some of settings can achieve for you. I'll review your comments and get back to you with questions I'm sure. Can you let me know if there's another way other than paypal to contribute to your you tube account. I had a paypal account at one time but it was de-activated as I hadn't had any activity on it for some time. 

Cheers!

[oldtbone55]

@daniel_lyall

Hello again Daniel,

I've got some questions regarding the changes you suggested.

1. Setup 1 2DContour 

I saw what you referred to and I entered a tangential extension in the setup of -0.300 to keep the cutter from eating material away from the heel. The cutter is now just removing material from 3 sides (the tenon) and not cutting into the heel. Is this correct?

2. Adaptives - tolerances

Are you referring to the tolerance setting under the passes tab that's at the very top? I should be changing this from 0.004 to 0.04? This only applies to some of the adaptives in Setups?

3. Setup 2 - 2nd to last Parallel Cut

I've adjusted the boundary cut by an additional 0.050". The cutter is now getting to the area you were pointing to. Is this the correct?

I've attached my updated file for reference when you have a chance to look at it.

Thanks.

[daniel_lyall]

---

@oldtbone55 wrote:

@daniel_lyall

Hello again Daniel,

I've got some questions regarding the changes you suggested.

1. Setup 1 2DContour 

I saw what you referred to and I entered a tangential extension in the setup of -0.300 to keep the cutter from eating material away from the heel. The cutter is now just removing material from 3 sides (the tenon) and not cutting into the heel. Is this correct?  YES

2. Adaptives - tolerances

Are you referring to the tolerance setting under the passes tab that's at the very top? I should be changing this from 0.004 to 0.04? This only applies to some of the adaptives in Setups?  Run the sim and if you see lots of tiny moves that does next to nothing adjusting the tolerance can stop them happening 

3. Setup 2 - 2nd to last Parallel Cut

I've adjusted the boundary cut by an additional 0.050". The cutter is now getting to the area you were pointing to. Is this the correct? Yep that's it, I was hoping blend was working in fusion this toolpath would of done a good job of cutting that spot but it's not yet.

I've attached my updated file for reference when you have a chance to look at it.will do

Thanks.

---

[daniel_lyall · Accepted solution]

It looks fine just change the tabs to triangular not rectangular. 

[oldtbone55]

@daniel_lyall

Hi Daniel, thanks for reviewing the file. I was having some funny toolpath crashes for some reason but it's all good now. I'm ready to do a test piece now and can't wait.

Thanks Again!

[oldtbone55]

@daniel_lyall

Hello Daniel,

For some reason I'm having problems with the toolpath in Setup 2, adaptive 10. Crashes are occurring due to collisions with the fixture. If I turn the fixture off and have just the body and solid stock turned I don't get any collisions. I've attached my file.

Thanks.

[daniel_lyall]

---

For some reason I'm having problems with the toolpath in Setup 2, adaptive 10. Crashes are occurring due to collisions with the fixture. If I turn the fixture off and have just the body and solid stock turned I don't get any collisions.

Its showing the crash when it's on as it's a defined object in cam (you have told fusion this is there basicly), so if the cutter only just touches it by 0.001 it will show as a crash as it's defined as a fixture and it's programed to not hit the fixture, it's fusions cam doing it's job.

Let's say If you have a vices on the machine or a fixture you set it as such (you can pick it in the stock tab as well ) and if the cutter hits it bang there goes something broken or worse, so it's saying this is in the way I will crash.

Now if you did not have it defined and the cutters goes into it the areas where the fixture or vise is it will crash straight into it as it's not defined as being there.

To get rid of the crash all you need to do is remove the material where it is crashing.

What I did was project the edges of the guitar body onto the bottom of the fixture/jig and extrude cut it away, I had to do a little bit of adjustment to it so it was not touching the jig/fixture, it only needs material removed where it is crashing.

Example attached

Daniel

[oldtbone55]

@daniel_lyall

Hello Daniel,

Could you take a look at the attached file? I've cut out the area of the jig where the crashes were occurring but I'm still getting crashes into the fixture and jig stock. I have one file of the neck where I'm not having any problems and this file is a replica of the one that's working but I'm getting crashes with it. I need another pair of eyes as mine are exhausted. Take a look when you have a chance.

thanks.

[daniel_lyall]

The crashes are the cutter just touching the jig in a few spots by 0.01in all you need to do is offset the sketch crash stock in by 0.05 then redo the extrude to the offset line.

To make it easier move the timeline to just after the sketch was done, do the edit then step forward to the extrude and reselect the sketch for extruding, it's fusion doing it's job showing where the cutters hitting the jig. If you look at the example I did you will see I had to do that myself.

It's just one off the improvements that has been made lately.

As you can see in the picks its just touching.

When these crashes show up in sim you can click on it and it will take you to where the crash is then you can just rotate around it to see where it's touching and just make a judgment call on it if it needs fixed or not.

[oldtbone55]

@daniel_lyall

Hello Daniel,

Thanks for your reply. I did as you suggested and increased the size of the crash stock to be removed. No more crashes! Thanks also for pointing out that by clicking on the crash in the sim it takes you to the crash site. I didn't know about that and was zooming in to the spot to see where the problem was. There, I've learnt something else from you. Now I'm ready to try it for real.

Cheers!

[oldtbone55]

@daniel_lyall

Hello Daniel, hope you're doing well. I got a chance to run the toolpaths for the neck yesterday. I had no problem making the fixture and doing the top of the neck but when I ran the last setup to do the bottom of the neck the program made the mill go down further at the tenon than it was supposed to and chewed away the material that was still attaching the tenon to the stock. I've reviewed all of the setups and checked the dimensions but can't figure out why this happened. I'm thinking this may have something to do with how the WCS's were configured in Setup 3. It looks like the bottom isn't the bottom of the jig but the bottom of the stock. Should I have used the jig bodywhen setting up the WCS's instead of the solid stock body? It looks like the cutter went further down than it should have by the same thickness as the material that's left on each end of the jig (0.190"). I want to try machining the neck again but would like to get a second opinion from you before I make any changes. I've attached the file that I used and haven't made any changes to it. 

Thanks for your help.