How to get 4th axis to 360° wrap around a part?

[Anonymous]

Hello Everyone, 

I am new to this forum and to using Fusion 360 and having a lot of trouble trying to get these two parts made.inner and outer transformer bobbins

Now these two bobbins where made on a lathe type mill for me by a friend but the lathe can't hold the tolerances needed as these two are practically rubbish. I have a Taig 4th axis mill and need to learn how to get this done in fusion 360. The new bobbins are smaller than these but in general look the same. I'll be using a two flute to rough out the part and a three flute for a finishing pass. 

The problem I am having is I can't get Fusion 360 to cut a single slot, and I can't get Fusion 360 to just clear off the stock to the right diameter before these cuts are to be made. Now being that I have a Taig 4th axis mill it doesn't have a lot of power so I can't just plunge in and then start cutting it has to be done in multiple passes.

Now manually I can start things off by measuring the stock diameter and then taking off a single pass at a time until I reach the correct diameter for the part but why can't I program this in Fusion 360? The 4th axis just has to spin around in a circle while the z and x axis move to cut the part out or is it more complicated than that? The stock is 2.75"Ø and cut to length. 

In my research I found this video on You Tube but I have no idea how this was done or how to apply it to what I am trying to do even though it is practically the same opperation: https://www.youtube.com/watch?v=YUgATlg9vW4

Any help with this is much appreciated. 

[etfrench]

The procedure shown in the video should work for you.  When you create the toolpaths for the grooves, use the multiple depths option.

This thread has info on how to mill the cylinder.

[Anonymous]

Thanks for the reply. I'm not a fan of sweeping it side to side as that wouldn't be truly round. I am trying to sweep a rectangle to a coil and then see if I can minus that pattern from the stock part and see if that will work. Fusion 360 doesn't work like AutoCAD and I am finding it a bit frustrating as I can sweep and line with ease in AutoCAD but haven't figure that out yet in Fusion 360. Even the move command is way different as in AutoCAD just pick the object, where you want it moved from and then where you want it moved to and your done. It took me forever to move the dxf part to the center of the stock body. 

I'll keep looking at that one video and see if I can figure out what he did with the plane stuff and unwrapping and rewrapping things. Sigh, I just have a lot to learn it seems so I'll keep at it and try to learn this system. I just wish the 4th axis stuff was developed properly for use as it really shouldn't be this hard. I can't even figure out how to turn my photo right side up as I tried but nothing seems to work.

[daniel_lyall]

It will help you alot to forget Autocad this is killing your fusion learning.

Go through this  https://www.autodesk.com/products/fusion-360/get-started

Then look through here https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-1C665B4D-7BF7-4FDF-98B0-AA7EE12B5AC2

The 2 links are the fusion learning you need to go through it so you can see where the differences are and it will show where you are going wrong.

The wrap function is a not on dead center operation it's slightly off, what Steinworks shows in the Vid is the way to do it, it is a completely well worked out work around that works. 

[Anonymous · Accepted solution]

Thanks for all the help everyone but know I am new to Fusion 360 not to drafting, designing, and troubleshooting, okay? as such I figured out a new way to cut a cylinder using Fusion 360 for 4th axis cutting. What I did to cut a cylinder was to create a square coil and then use 2D contour on that square coil to generate a good machine path. I already know that the side to side method will not give a good surface finish so if a good surface finish is desired then this is the way to go.

With this method you must know the tool's speeds and feeds as those specs will be used in the creation of the square coil and in the multi-passes when setting everything up. The radial depth of cut for your tool will be the selection size of the square coil and the axial depth of cut will be used for the multi-passes. If you mess this part up more than likely you will end up breaking the end mill. Choose a turn count that doesn't make the tool to come in to harsh for the square coil you will be able to see this on the simulation.

To get it to cut to the desired diameter you simply take the selection size and add that to the desired diameter you wish to be at when creating the square coil. Then the rest depends on the tools requirements for feeds and speeds. 

As I begin to learn Fusion 360 I'll try and pass on the need to know information to help others as I learn new things that I figure out along the way. 

[etfrench]

Looks like a nice way to get a smooth cylinder or a cone.

[daniel_lyall]

If you do a project - include 3D geomentery of one edge you can get a single direction.

[Steinwerks]

@Anonymous can you share the part here? It can be difficult to troubleshoot toolpath issues without an example to work with.

[Anonymous]

I'm not sure how to do a "Project" on this and since it is wrapping the part not sure of anything 3D will work. I'll give it a try and see how it goes 

[Anonymous]

I thought I did share this part in my first post in a dxf file. This one is the EC 90 Primary Choke bobbin. Is there another way to share this that I might not be aware of? Basically I draw these up in AutoCAD and save them in a dxf file and download that file to Fusion 360 and start working on them. I've been working with AutoCAD since 2006 and am comfortable with using it but I am going through a lot of Titan's videos so I can learn more about Fusion 360, as well as doing a lot of research on the internet. 

[Steinwerks]

You can export your existing work as a .F3D which is much easier, since then we'll be looking at your model as you have it ready to go.

https://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How...

[daniel_lyall]

Sketch menu - Project - include 3D Geomentery 

.

j

[Anonymous]

I'm not sure if I did this correctly so let me know if that is what you are asking for, okay?

[Anonymous]

Wow! I'll have to give this a try for sure. Thanks

[Anonymous]

I got the new line but what did you use to create the tool path?

[daniel_lyall]

2D contour set up as a wrap toolpath with leads turned off and useing ramp example attached.

[Anonymous]

Okay, I think I'm not getting the projection part which is why when I try to generate a tool path it fails. Can you walk me through that process as I keep creating a sketch for some reason and it doesn't seem that you are creating a sketch. 

Wait I think I got it. But when I checked the machining time it was 1hr 51 minute compared to 1hr. Not sure where the extra 51 minutes came from as there seems to be less wasted movement the way you did it? 

[daniel_lyall]

It's the ramp doing it (the ramp feed rate as well) if you can enter from the outside and exit from outside you don't need to ramp,it drops almost an hour of the cut time with no ramp.

One question why the tinny tool.

The ramp feed rate can be the same as the cutting feed rate most times depending on the material. 

[Anonymous]

Yeah, I took a look at it and will change to a larger tool for the first few operations as only on the inside of the thin walled places do I need the smaller tools. These thin wall places are very hard for a lathe to do as the blade will walk trying to cut that deep. I have been changing things around but for the most part I just needed to learn how to get 4th axis to act as a lathe as on a part such as this a lathe can't hold the tolerances. 

Today I plan to learn how this was done in this video https://www.youtube.com/watch?v=YUgATlg9vW4&t=9s as when using the square coil method I can't go to the sides on the second operation as that would crash into the walls so I need to clean up the sides after the second operation is done and then get to those thin walled cuts. So, I will be using a 1/4" tool for the first two ops and then switch to a roughing one or two flute end mill and finally to a three flute end mill for finishing up the part.  

[daniel_lyall]

Thats where I learnt this sort of thing from.

One thing that would work is to run mist coolant with the pressure turned up and haveing the air compressor sitting somewhere cold.

This will do two things blow the chips away and keep the part cold.

When cutting Plastic a single or double O flute is what's recommended as they get the heat and chips out fast.