Cutting Splines With Single-Point Thread Mill 4th Axis

[Lars2024]

I would like to cut some splines into a round part. I made the profile of the splines to match my single-point thread mill. I imagined having the cutter go to the far side of the part on Y, going half of the diameter down in Z and then making a cut while feeding in X. Ideally, I would like to have some roughing passes. I have about 50 splines around a 0.650" cylinder. These splines are very narrow and only a few thousandths tall.

I have tried everything I could think of, all with no luck. I eventually gave up and changed the angle to a 45 degree so I could use a form mill to get the job done. I couldn't get the Z-axis to properly get set for tool orientation, the Z wanted to go through the centerline of the part every time.  It doesn't help that with the recent update of Fusion 360 it crashes all the time with almost no pattern to it. It might be time to give that guy from Esprit a shot. Fusion has been very tough when it comes to 4-axis work so far. If anybody could give me some help I would very much appreciate it.

Thanks! 

[seth.madore]

This should just be a simple 2D Contour toolpath with Roughing Passes enabled. With math or physically measuring the tool, we can get to the centerline of a threadmill, so we would plug that value (once we know it) into our Bottom Height Offset. Alternatively, we could also give it a negative Height Offset adjustment at the machine..

WCS needs to be set to centerline of rotation.

Any chance of seeing the part and understanding what tool operations you were trying to utilize?

[engineguy]

@Lars2024 

Sounds like you were not far off, only issue seemed to be where the Z axis was plunging, I just tried to do it with a single point thread mill ant it doesn`t like using Contour, tool shows Red which means it is the wrong type of tool so I used a Trace strategy and it works fine, the issue with the Z plunging into the middle of the stock can be adjusted using the "Sideways Compensation" under the "Passes" tab, if you are starting at the right side of your stock looking from the front (-90) the to move the tool over select "Right- conventional" and it should move your tool over to the right, seems to work here anyway!! Don`t know if this is the right way to do it, but it is at least a "workaround"!!

Personally when I do any splines I always do it from the top using something like a 45/60 degree chamfer tool or if I need a special shape I get a tool ground at a tool grinding firm locally, they have all the proper gear and not too expensive!!

Anyway, screen cast below for you and file attached, I went a bit overboard, ended up with 450 splines round a 60mm bar!!!

!!! What gives, can`t insert a Screencast, everything has changed, including how to get a file and upload it, are they monkeying around with the Forum???

Hey guys, it wasn`t broken so didn`t need "fixing/breaking"!!!!

Screencast link maybe!! https://autode.sk/2PEvv2i

Regards

Rob

[Lars2024]

@engineguy  @seth.madore 

Thank you for taking the time to give me some help! I was able to do this with a tracing method and a contour. It was a HUGE pain to figure out how to get the Z-axis to orientate correctly (Which will get the A-axis in the correct orientation). Let us not forget we are working with a cutter that has an angle on it. I had to make a small flat on the top of the splines then I had to do some work in the surface environment. I made an "imaginary" flat to properly orientate the Z-axis (for the tool orientation) so that the angle on the tool matched up with the angle on the part. Is this the 4th axis type of work that everyone is complaining about with Fusion 360? 5-axis work is all fine and dandy, but not indexing in 4th? Did I miss something? I know that someone out there can figure this out much quicker than I can. It goes without saying that I burned a ton of time that I could have spent doing something more productive. I have attached the file, hopefully this helps the next guy who tries something like this in the future... or Autodesk could help us out in the next update *hint* *hint*. 

Thank you again @engineguy  and @seth.madore  for taking the time to give me a hand!      

[johnswetz1982]

Once you have one toolpath that works, put that into a circular pattern of however many you need and you should be fine then. 

[engineguy]

@Lars2024 

Looked at your file, possibly one of the reasons for your confusion was the orientation of your drawing, the way you had it drawn made it quite hard to visualise the orientation needed, the Trace works best in my opinion if just doing the cut in a single pass, however as you have found if you want to do multiple depths best to use the Contour as it give you that option.

I have moved a few things around in the file I am uploading for you just as an example of how easy it can be to use 4th axis indexing, I think that a lot of people do have problems with getting the setups done, especially those that use the "Y axis up" orientation.

I always create my model if it is to be machined exactly as as it would be in the CNC machine.

Anyway, have a look just for interest 🙂

Regards

Rob

[Anonymous]

I had issue with key cutter definition and new tool library, crashed few times.

Tool runs in simulation but will not post so I gave up on that, flat end mill does post with Haas 4th axis.

Model has some issues with edges of splines floating above cylinder, not joint at edges, needs rework. 

Take a look at sketches, I used lines drawn at 90 degrees to spline front edge as tool orientation for flat end mill and another line for key cutter.

I tried to come up with process that works and I think this has some potential if you can polish out the errors with model and key cutter.

[Anonymous]

Update, reset patterns for less A axis rotation back and forth, fixed key cutter error.

End mill cuts all splines in one direction then in the other direction.

[Anonymous]

Little bit of cleanup work done, corrected tool orientation for key cutter and deleted planes and sketches used in exploring.

[Anonymous]

Trace tool path added to top of splines, almost good enough to push cycle start button.

[Anonymous]

Rob, I took  closer look at your file, idea seems attractive, but are you aware of the fact that tool is out of sink with spline angle ?

Left screenshot shows thread mill tool from your file and right screenshot shows end mill from my file, both in same view with stock set to transparent.

You need a sketch defining tool orientation relative to geometry being cut.

I fixed it but it needs rest of the work done, also in my file, I used contour with wear compensation instead for fine adjustment.

Here is a screenshot of proper alignment of thread mil, modified file attached.

[engineguy]

@Anonymous 

Hi Vic

Wasn`t my file, I just did a little "house keeping" on @Lars2024  file, I would have liked to have had the time to start it from scratch and also personally I would not have considered doing the splines in the manner it has been done.

I would have done it from the top with a tool ground to the shape required which alleviates a lot of the issues in the OPs original approach to the job.

Regards

Rob

[Anonymous]

---

Sorry, I had no idea, just wanted to draw attention to discrepancy. I've  seen a few cases where OP gets in with some "issue" and runs off to sunset without much interaction.

So maybe this is just a tool for decorating pizza or pie doe edges and nothing bad will come out of it.

My first thought was ,......... "what's wrong with standard end mill?" so I was curious how it would work out and first thing I saw was floating splines on cylinder,.... I think I got the concept down even with out fixing model, just wonder what OP ended up with.

[Lars2024]

I am working on this right now. I'll keep everyone posted. Part of the reason the model was so "broken" was because I had to delete a ton of the other features (and the timeline). This is a part of in-house tooling and a "trade secret" for my industry. I will let you all know how I make out.

[Anonymous]

Oh there you are, you may have noticed that I completely ignored cylinder and used base edges of splines to machine space between splines using key cutter. The space is only .03 wide so if you had model showing circular surface connected to spline edges, wrapping tool path around such a narrow space would require something like .01 diameter end mill to show any effect.

Key cutter or slitting saw seems like the only logical solution to me.

[Lars2024]

After some redesigning of the part to better cater to the tooling I had in the shop I was able to get this tool made and the customer now has a line up and running.

I didn't expect to get that much help and so quickly! Thank you all! 

@engineguy  You helped me to get this going in the right direction and gave me some great tips! Could you please give me the company information for the cutter grinding firm you mentioned? 

@johnswetz1982 Great tip on the circular pattern. This is a no-brainer type of feature and will save me lots of time down the road. 

@Anonymous Great tip on using sketches to properly orientate the tool. That is not something I have ever had to use but it helped me dramatically in this job and I will keep that trick up my sleeve for future reference. 

You guys are awesome! 

I am pretty disappointed with Fusion 360 when it comes to 4 axis work. I had too many issues with trying to get the cutter to line up and get a toolpath that didn't want to dive into my solid model or just not want to touch it. For whatever reason, the 2D and 3D contour wanted to go much further than what was selected. I tried all sorts off different sketches and tried anything I could using the patch environment. In my honest opinion, there were way too many workarounds, tricks, and manipulation of the model/sketches that needed to be done to get a good tool path considering what needed to be machined. 

I like Autodesk and Fusion 360 as they have been very good to me. There are all sorts of helpful information and tutorials available for when you are having a tiny issue or when you are really "in a jam". The CAM side of Fusion 360 has just consumed WAY too much of my time and I think it is time to look at something else. I am looking into Esprit, Mastercam, and some other Autodesk products such as Feature CAM and Powermill. for what its worth, I like Fusion 360 on the CAD end of things, it has a learning curve and some strange caveats like any other CAD software but it is my favorite CAD software of all time. There is something to be said about the Autodesk community when you look at how many responses I got and so quickly.    

[engineguy]

@Lars2024 

Nice to see such a well balanced reply at the end of the project and very glad that you have been able to satisfy your customer and (Hopefully) get paid!!

As I am located in the North West corner of England I doubt that the grinding company we use would be of any help to you as I think you are quite a long way away 🙂 🙂

P.S. If you do move to another Cad-CAM system I have used both of the Delcam products you mention and although it was a long time ago (2004) when I last used FeatureCAM I found it to be very, very good even way back then and as for the Powermill software that is really awesome !!

Downside neither of them are cheap nor is MasterCAM but for pretty good CAD but superb CAM then yes, go for one of them, as you rightly point out that while Fusion 360 is great for CAD the CAM is no where near as mature as those others!!

I don`t know if you have tried it but the other online CAD I have had a go with is Onshape, quite different and interesting if you have the time, I don`t so have only scratched the surface on that one !!

Regards

Rob

[Anonymous]

Party time,..... whenever you don't have model edges or faces to use in setup, as cutting geometry or for tool orientation, create sketch.