Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Path that uses the side of the tool

mbradleyDDG6T
Enthusiast

Path that uses the side of the tool

mbradleyDDG6T
Enthusiast
Enthusiast

I'm looking for a tool path that will allow an endmill to cut using the side of the tool in the z axis while moving in the x axis.  depth of cut to finish at .03 in the y in an up/down zig zag path.  Any suggestions?

0 Likes
Reply
736 Views
14 Replies
Replies (14)

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

The 2D Contour using Ramp will move down in the Z while cutting with the side of the tool when moving in the X/Y direction.

Or, the 3d Contour.

 

Always easier if you upload a Fusing file so folks can see exactly what you are trying to do, the above is just guesswork !! :slightly_smiling_face: :slightly_smiling_face:

 

To upload a sample Fusion file go to :-

File > Export > Select f3d format > Save to a location on your computer > Then attach to your reply.

2 Likes

mbradleyDDG6T
Enthusiast
Enthusiast

I've attached an F3d file for your viewing pleasure. Also, if you look about 3:00 min of this video it gives an example of what I'm trying to do.  https://www.youtube.com/watch?v=rdciRX0lol0

0 Likes

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

The Trace is probably the best option, see image below and attached file.

 

Blank Slide.jpg

 

 

1 Like

mbradleyDDG6T
Enthusiast
Enthusiast

Greetings Engineguy,

It's interesting, if you look at all the paths I tried, Trace was one of them and oddly enough it would not work, yet now it does, is this typical that Fusion can have a "change of heart" so to speak?

0 Likes

mbradleyDDG6T
Enthusiast
Enthusiast

I take that back, when viewed from the side all seems well and good, but when viewed from the front it becomes clear the tool is cutting into the model beyond the .03 depth of the feature. Any way to fix that? I tried setting radial stock to leave to various positive and negative values with no affect.

0 Likes

mbradleyDDG6T
Enthusiast
Enthusiast

Greetings Engineguy,

For some reason I cannot open the file you sent back to me, Fusion is telling me "you are in the process of installing an update that is required to open Untitled" any idea what that means?

Thanks

0 Likes

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

Current Fusion version is 2.0.11894, the file I uploaded is not named "Untitled" so no idea what you are trying to open.

It is all about selection, select edges as shown by holding down the "Alt" key and picking one at a time, then set the Compensation to "Left" and then set the "Stock to Leave" to the -0.03in offset and preserve order, works here, see images below, very easy :slightly_smiling_face:

 

Blank Slide-3.jpg

 

Blank Slide-2.jpg

 

0 Likes

mbradleyDDG6T
Enthusiast
Enthusiast
Good morning Engineguy,
Today the file you sent to me will open, not sure why, but your answer worked pefectly, thanks again for the help!!
0 Likes

mbradleyDDG6T
Enthusiast
Enthusiast
One other question, your solution to my question works perfectly, but how did you arrive at that answer as I do not find it to be intuitive. Is there some resource that explains a strategy or is it all by trial and error?
0 Likes

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

OK, your question is "how did I arrive at the solution" correct ??

 

First of all I had to decide which toolpath to use, as it is a "rising/falling" operation then that meant I needed a toolpath that will follow in 3 axis, answer, the Trace toolpath.

Next, how to get it to work, need to know how the Trace works, so, I know that it defaults to "Center" which has the center of the tool running on whatever edge/line is selected, this means that the tool cuts too much away so I then choose Left Compensation which will move the center of the tool over by the Radius of the tool, this now means that the tool will miss the selected edge/line as the side of the tool is now at the selected edge/line, right, now I have to bring it back the correct amount for the edge of the tool to be the correct distance in, simple way to do that is to check the depth of the pockets which turned out to be 0.03in, so, now I have to move the tool over by the 0.03in so an easy way to do that is to use the "Stock to Leave" facility and instead of telling it to leave a Plus stock amount by inputting a negative value will move it in by the set amount, that is the -0.03in "Stock to Leave", and that is all, everything is very simple but it obviously requires knowledge of how certain things work :slightly_smiling_face:

 

Is it "intuitive" ??

I would say yes it is, Trace defaults to Center, to move it use either Left or Right Compensation to put the edge of the tool on the selected edge/line, to then offset the tool either in or out then the Plus/Minus "Stock to leave" is the most obvious choice for simplicity, that is it, IMHO very easy :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

Hope that makes things a little clearer for you.

"Clarity is King" :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

1 Like

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

P.S. Hope the above was helpful, I see many people using Sketches to try and get the tool in the right place but one thing to always try to remember is that Fusion 360 is a Parametric Solid Modelling software so always try to use the actual Solid that you have modelled.

The user should also try to create the Model as it will be machined, for example I see people all the time doing Pockets with 90 degree corners in the Model and then using a 1/2in End Mill to cut it out, poor practice, as when it has been toolpathed the tool will have no Fillet to go round and will be just running to a sudden stop and then changing direction, if a 1/2in EM is used then there will be a 1/4in radius in the corner of the finished part, so why not Model the radius in there to start with ?? Preferably slightly larger than the radius of the tool :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

 

All about Product Knowledge, Machine Knowledge, Material Knowledge and most of all good basic Engineering/Machining Practices :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

0 Likes

mbradleyDDG6T
Enthusiast
Enthusiast

Good afternoon Engineguy,

I should mention, I'm not a machinist and I'm trying to learn as much as I can about this world of CAD/CAM with Fusion 360, I've been at it for about a year now and the learning curve has been rather steep.
I do appreciate the "clarification" but I must explain what I mean when I say it is not "intuitive" by its nature and here's why I say that. I do understand that Trace is by definition a tool path that traces a contour with varying z, but in the description, while it does mention right and left compensation it is not clear what that means. So, in the "Passes" when it mentions left or right compensation, it does so in the context of climb vs conventional milling and only only vaguely mentions the tool being offset from the centerline, couple that up with the option of choosing either single contours or multiple contours, having a left or right comp may in fact not give the correct tool path. In my case, I chose the "bottom" contour line vs the top contour line and regardless of the amount of stock to leave, the tool path would either give me a warning that the stock to leave was incorrect or it was clearly cutting into the model beyond the contour of the feature I was attempting to machine. Anyway, all that aside, I am grateful and thankful for your help. 

 

0 Likes

engineguy
Mentor
Mentor

@mbradleyDDG6T 

 

Well, I can only apologise if I am unable to clarify the issue, the word "compensation" used in the context of CAM toolpaths means there will be an "offset" to one side if there is a "Sideways Compensation" applied to one side, this is uaually the Radius of the tool and goes all the way back to the days of only Manual Machines and is a basic of all machining.

 

For your part I am able to use the inner edge selection and use either the Left or Right Sideways Compensation and by using the inner edge the "Stock to Leave" is actually not required so I only needed it because I used the outer edge, which, in fact was not the easiest method, my apologies for that :slightly_smiling_face:

Leaving the "Sideways Compensation" at the default Center will not work because if there is no compensation then there can be no Plus/Minus "Stock to Leave" :slightly_smiling_face:

 

How are you selecting your edges to toolpath ?? The best way for such an operation is usually to "Hold down the Alt Key" and select edges in the order to machine and then use the "Preserve Order" which does exactly what it says it does :slightly_smiling_face:

 

I do understand that not every persons brain works the same but these things are very basic and yes, I know it is a very steep learning curve but the basics of anything have to be mastered pretty early, the software is what it is and works fine for many thousands of users, and yes again, the "terminology" can sometimes be a little confusing especially for first time users of a CAM software, older folks will likely have experience of other CAM softwares so are able to "read between the lines" and understand more easily what is going on that`s all :slightly_smiling_face:

 

Yes, Fusion does have it`s faults and quirks but it is very young compared to the majority of CAM softwares currently available, it is only what around 5/6 years old I believe ? Others are more than 30 years old so thinking ahead what will Fusion be in another 25 years or so ???

Hopefully it will be incredible but I am unlikely to be around to see it, enjoy :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

 

1 Like

mbradleyDDG6T
Enthusiast
Enthusiast
Hey Engineguy,
Sounds like you and I might be of the same generation, but here's the way I see it, this stuff has to be dumbed down to the lowest common denominator,,,, me...
0 Likes