My last attempt to generate toolpaths before I uninstall.

[Anonymous]

Ok I am at the end of my rope. I am attempting to generate toolpaths to cut out a Les Paul guitar from STP files I bought on GrabCAD. I have been met with frustration every single step of the way and I'm very close to throwing in the towel and moving to Rhino or Solidworks. This is about the third time I have had to post here to get help generating tool paths. I appreciate the help, believe me, but I can't work like this. I watch Lars and NYCNC Fusion CAM videos all day long and it looks so easy in the hands of someone who knows what they are doing, but as soon as I try something as simple as drilling a hole for a switch....nothing. I can't even select the geometry. It makes no sense. The CAD part of Fusion makes sense and I like working with it, but the CAM makes me want to throw my keyboard through my monitor.

Today's abomination revolves around trying to route cavities for pickups and simple holes for a switch and volume/tone pots. On the PU cavity I have tried 2D pocket, 2D adaptive clearing, I think I tried 3D adaptive as well, but I get more or less the same error:

"Error: Unsupported geometry for 2D Open Pocket detection!"

For the holes I can't even select the geometry. Not the bottom edge, not the top edge, not the sides of the hole, nothing. I have been using the "isolate" command since it was suggested here several operations back, but it is not working for these two operations. For the holes I tried "bore" and "circular" under the 2D menu. "op 14" is the pickup cavities, and "op 15" is the holes for the switch/pots.

[jeff.pek]

Sorry you're having trouble. There was a recent thread on pros & cons of converting mesh models into solids. You've found one of those situations. Mesh should work fine with 3d operations, but not for 2d operations like drilling. I think you'll probably benefit from converting the mesh bodies into solid bodies in CAD first, before you start to do operations like that in Manufacture.

Happy New Year.

Jeff

[tmostad]

I may be out of my depth here and if so then I apologize in advance. Anyway, I took a look at the geometry for the tool paths that show the errors and I can see gaps in the selected geometry (blue lines around the pockets). If you look at the Right view for the TopCap Crave for the last op, "2D Pocket10", you will see that the pocket is not confined to the X/Y plane. You need to change your WCS to be valid for the pocket bottom if you want to use a 2D pocketing op.

[Anonymous]

Hi Jeff, and tmostad,  Happy New Year to you too!

 These files were purchased from Matt Meyers on grabCAD in the interest of saving time and I figured I wouldn't do a better job creating the CAD model than Matt anyway. I'm not sure about some of the gaps in the edges as I didn't do the original CAD, but I notice this when trying to select the bottom of the pickup cavity which as I understand it, would be the geometry to select in order to machine out that pocket.  The author of the files broke each machine operation down into a separate STP and IGS file. I imported each STP into a separate component as advised on an earlier thread here.Even so, and with isolating each "operation" component, in the case of the pickup cavities, earlier operations still show such as the diagonal wire channel running from the pickup switch cavity to the control cavity. The neck pocket also still shows up.

I will look into converting the meshes into solids in CAD and the WCS.

[tmostad]

Here is a toolpath generated by setting the WCS to match the bottom of the pocket and selecting the pocket boundary (yellow lines) then setting the depth to selection and choosing the pocket bottom. Obviously it needs more work but it generated a toolpath. Note that since the pocket bottom is not in the same plane as the guitar top surface, you will need to mount the body at the proper angle before machining. Or you could modify the design so that the pocket is in the same plane as the default X/Y plane.

[tmostad]

As I look at it a bit more, there are at least two different planes that are used for geometry so modifying the pocket bottom is not really an option. You will need to determine all of the geometry for the various planes and mill each in a different setup mounted normal for each plane. You can easily see the different planes by looking at the Right view for the guitar. BTW - I looked at the model a bit and I can find no problems.

[tmostad]

Just for fun I measured the angle of the plane through the bottom of the pocket and it is 4.2 degrees per Fusion 360 from the plane on the bottom of the body. The length of the body is about 440mm which means if the rear of the guitar is flat on the mill then the front edge needs to be raised by about 32mm when you mill the pocket bottom. Please verify these numbers yourself.

[Anonymous]

Thank you again for your efforts!

Just for some background as to why there would be an angled bottom to the pickup pockets, on Les Paul guitars the neck pickup and the neck pocket are set to a 4.5 degree angle relative to the plane of the body. On Fender guitars like the Stratocaster, there is no neck angle and they used "string trees" on the headstock to apply the necessary downward pressure on the strings after the nut. Gibson guitars were built in a more traditional manner with the neck set back at a shallow angle from the body and the headstock set back at a further angle to achieve some string height above the body, and downward pressure at the bridge, a good playable action on the neck, and downward pressure on the nut for proper sound.

I can't tell from looking at the model whether Matt designed this 4.5 degree angle into the neck pocket and pickup pockets. If he didn't I will have to modify the CAD drawing to put that angle in there.

So you can also select the top edge of a pocket and then set the cut depth to the bottom of the pocket? I didn't know that. I thought you had to select the bottom of the pocket. I have a lot to learn about CAM. Cad is easy by comparison.

[Anonymous]

I tried to convert the meshes to "breps" according to this article, but once again I cannot select any body. I click on the body in the project window, I click on the components in the tree, and nothing.

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-t...

[engineguy]

@Anonymous 

I thought you said at the start that you got STP files, if so then no problem, the issue is that as has already been noted is that everything is at some kind of angle and are next to impossible to machine on a 3 axis cnc without spending many, many hours doing many angled setups, for example, the 4 holes for the control "pots" are all at angles to the curve of the top face and will require 4 different setups just to do those 4 holes !!!

What version of Fusion do you have? Is it the "Personal" version ?

Stay Safe

Regards

Rob

[seth.madore]

If you also have these in .igs format, that will be the better option

[Anonymous]

The truth is your problems are sum of arbitrary activities that don't add up to anything solid, so let me point out few things to set you on the right path.

1 - Do setup for each segment of machining by selecting Z and X orientation referenced to model faces, edges or sketches.

2 - Select only bodies you intend to machine in that setup.

3 - If you are using model as stock, make a copy and defiture it by deleting cavities, pockets or holes from it.

4 - Set origin in Fusion and in your machine at same location on model or stock, something that you can easily establish at the machine.

5 - Machine only those features that are in sink with how your machine kinematics work, so in case of drilling holes, holes must be in line with Z axis, in setup and in machine.

As you can see in screenshot, I used tool orientation to drill one hole just to show that holes are at angle and that's why you cannot select faces.

So, if your machine cannot tilt Z axis, you will have to tilt the model in setup and in machine.

Looking at Contour toolpath, finish is a "little bit rough", may wanna try few levels of increasingly smaller stepover, finishing with Parallel strategy.

I wouldn't rush with uninstalling Fusion, instead, put some work into building your skills from simple projects up.

[tmostad]

How you approach CAM has a lot to do with the way the model is created and which operation you are trying to choose. Sometimes, in particular for simple, regular pockets on the normal plane, picking the bottom of the pocket will work. In your case the pockets are irregular with different levels and outlines so you have to help it a bit more. Picking the boundary then the pocket bottom is a way to help the CAM figure out exactly what you want to do. When CAM tells you that it couldn't generate a toolpath it doesn't necessarily mean that there is no possible toolpath with the parameters you chose. It may mean that there are ambiguities that prevent it from knowing the right choice among many so it gives up. You then have to sus out why. It can be mystifying at times, even for experienced users. It think it is important to believe that the CAM in Fusion 360 is pretty darn good and if you are not getting the result you want then continuing to look at the problem is worthwhile. And when that fails, posting here can be helpful too.

[engineguy]

@Anonymous 

Here is a simple example of what you are going to have to do if you don`t have both a 5 axis CNC capable machine and 5 axis toolpaths available in Fusion or any other CAM software !!

This is your top part set to the 4.5 degrees that gives you the vertical walls for these pockets so they will toolpath and cut correctly, that is the only way you can do your project using only 3 axis CNC Machine.

Have a play around with it to get the idea, if you look at the 4  control "pot" holes you can see that you would have to do 4 individual setups just to drill those 4 holes, they are all at different angles in both the X and Y !!

Example file attached.

Stay Safe

Regards

Rob

[Anonymous]

Ok I'm going to reply to everyone in this one post.

Rob, I have the startup (entrepreneur) license. The gabCAD files came in both STP and IGS. I imported the STP files into Fusion. Seth your suggesting I import the IGS instead? I will try that in a new version while keeping the one I'm currently working on.

Rob, regarding the separate setups for the angled holes, could I do the hole bore operation first while the stock is still flat before doing the profile carve? The inside pockets that will contain the switch and control pots also have angled bottoms. Those are machined from the back of the guitar. As these are inside pockets and not visible on the finished instrument, I'm not concerned with scallop lines showing in the finish. Do I really have to angle the stock so that the stock is perpendicular to the Z axis for the angled cut? I would think the CNC could still carve a pocket with an angled bottom with the stock flat to the table. Even if the finish is not perfect, it's ok. If that will not work and the actual hole needs to be angled and not just the top and bottom surfaces for the installation of the hardware, I could make a jig and just drill them by hand. The hole is just for passage of the potentiometer's shafts and switch toggle. As long as the surfaces that hold the body of the device and their coresponding nuts are at a matched angle, the actual angle of the walls of the hole won't matter as long as it is big enough to let the shaft pass through.

VicKosta, what you suggest is what I have been trying to do by importing each STP file which contain a separate machining operation, into a separate body, then isolating each body and doing separate setups. The problem is even with isolating, previous geometries are still visible in certain circumstances such as the pickup pockets. The angled wire channel and neck pocket still show up. This must be because the original stp files despite being separated by operation, must contain more than just that operation's geometry so isolating doesn't get rid of the other channels and pockets. I haven't tried copying and then deleting the other stuff.

  A Les Paul is a complex project, but I have a client who is ordering two of them and I want to utilize CNC as much as possible.  I bought the CAD files instead of drawing them myself trying to save some time.  This particualr project is the most complex thing I have attempted in Fusion to date, but I have had issues with CAM in Fusion from the beginning. If anyone can suggest a good course specifically on Fusion CAM I am all eyes, as it were. One geared toward woodworking would be even better. There is a lot of information out there on CAD, and I have a reasonable handle on that. CAM on the other hand is bewildering.

[engineguy]

@Anonymous 

Seth is right, the .IGES files are usually better to work with than the .STEP files, depending on the software used to create them, example if the original files have come from Solidworks then go for the .IGES files, their .STEP files are not the best in my experience anyway 🙂 🙂 🙂

Yes, there are a few operations that you can do with the piece flat on the table and yes again for being able to do sloping floors to some pockets, no problems there, you can use whatever fine stepovers you need for the finish you want, the big issue is with the pockets with the sloping walls, they could be done with the piece flat using 3D toolpaths, but they will have an "undercut" if the piece is flat so you would have to use something like a radiused "Slot" mill or a "Lollipop" type mill that would get under the angle enough to clear out the pocket and give you the angled walls

Basically, you have really "bitten off a chunk", if I was doing that job I would be going round to a friend of mine that has a nice big High Speed 5 axis Router that has a Tilting/Swivelling head and just throw the G code at him and a few pieces of material and he would likely turn it around in a couple of days or so, might be an idea to ask around at some other shops, could actually work out cheaper for you 🙂

If you have the "Startup" version then you will have acces to some 5 axis toolpaths and most importantly you will have "Tool Orientation", that will allow you to toolpath any and all your of your project parts quickly and easily, plenty of 5 axis Post Processors to choose from that will/can be made to suit a 5 axis CNC so you should be able to create the G code needed for most any machine 🙂

Or really "push the boat out" and buy a B and C axis Head for your machine, might be good investment for the future 🙂

Anyway, from all the excellent information from all the other folks you should get there in the end, if you keep having to come back with individual bits that aren`t working for you then feel free, as you have found the CAM is in a different Galaxy "far far away" 🙂 🙂 🙂

Stay Safe

Regards

Rob

[Anonymous]

On subject of IGES files, I had numerous files supplied by customer in that format, many had overlapping surfaces that had to be trimmed or double surfaces that had to be deleted before stitching file into a solid body and I always do that so that I can cut body and not see hollow inside before moving onto programming any tool paths.

So, where does one benefit from IGES format vs STEP?