3D Contour containment - how to avoid stock

[Muzzerboy]

I'm hoping to use a contour tool (like a "slot" or woodruff tool, with a rounded nose) to cut cylindrical slots in a cylinder, parallel to the axis. This will be repeated 32 times around the circumference on a 4th axis, to form an HTD timing pulley.

I've created the tool OK and I generated the model easily enough. I've tried pretty much all the toolpaths that appear to support this operation (which seems to boil down to just 2D and 3D Contour) and the only toolpath I can get to machine out the slot is the 3D Contour (the 2D Contour had a go but missed much of the material and removed other stuff it shouldn't). It appears to do a good job of the slots. However, I can't prevent the tool from plunging in to the stock at either end. At the free end of the bar stock it probably isn't an issue but at the clamped end, it certainly would be(!)

There don't seem to be any options for controlling the lead in and lead out that would prevent gouging. Ideally the tool would approach the stock from outside, rather than plunge down inside the stock first. The screenshots show what I mean.

Can somebody either suggest a way to get the toolpath to behave or failing that, suggest a different solution. I'd like to use a disk-like cutter rather than a ball end mill but either way I'd like to understand how to control the toolpath in this context. Surely it must be possible but after an hour or so I've run out of ideas.

I've searched this forum but couldn't see anything that helps. Model attached.

Thanks

[mailRQAJW · Accepted solution]

@Muzzerboy 

Is this a bit closer to what you need? Modified file attached, mostly it is the Leadin/Leadout that needs sorting, and fine tuning the depth of cut using the - (Minus) Stock to leave, should be fairly close I think, or maybe just of use as a pointer, if you don`t want the little radius at the end of the slot then play around with the Tangenital Extension Distance setting, I changed it for image 2 to -4.25mm, ie Tool radius, you can move the end of your slot to be shorter/longer by using this option.

[Muzzerboy]

That looks encouraging. I tried various positive and negative angles and distances but must have missed that combination!

I'll take your settings and have a play with them. It certainly looks pretty close to what I'm after. There seems to be a way.

Many thanks - I was sure it must be possible but I guess it was hiding in plain sight!

[Muzzerboy]

Well I've got the 2D Contour toolpath working now but it's a bit of a fiddle really. You have to play with both the radial and radial stock to leave settings until it "looks" right in the simulation view, which doesn't sit well with me as I prefer to see an analytical solution.

It's tantalising that the 3D Contour seemed to generate an almost ideal toolpath directly without the need to mess about with offsets. Using the correct tool radius, it seemed to place the toolpath exactly where it needed to be. The fly in the ointment was the lead-in and lead-out which caused a terminal clash with the stock and didn't seem to be configurable. It feels to me that with a bit more control of the lead-in and lead-out, the 3D Contour would be by far the best solution.

As another option, it looks as if the "trace" toolpath may offer potential, although again it looks as if it also requires a lot of trial and error with offsets, tool angles etc which feels like a bodge job to me - not what CAD/CAM is about surely? However, at least it seems to offer more levers. Here's an illustration of what can be done although I haven't had a go at seeing what my job would look like in this scheme, as I have a life to live:

https://www.manandmachine.co.uk/fusion-360-cam-cutting-axial-grooves-on-a-turned-part/ 

[mailRQAJW]

@Muzzerboy 

No, you don`t have to "fiddle around" as you put it with the 2D Contour, easiest way is to just Sketch a line where you want the tool to cut to along the groove, if you are going to do the cut in a single pass then you only have the Bottom Height to set, if doing more than a single pass then easy enough to use the "Roughing Passes" option in Contour to cut the groove in smaller cuts.

As for the Leadin/Leadout if you want to approach the stock in a straight line then just set the Horizontal Radius to 0 and the "Lead-in Sweep Angle" to 0 as well, then set a distance that you want to start at from the Stock. For the Leadout again set the Horizontal Radius to 0 but leave the "Lead-in Sweep Angle" at 90 degrees and a distance to move away from the stock at the end of the pass.

Anyway, see the attached file and FWIW if I was doing this job I would simply have a Tool ground to the shape of the groove, cost is minimal compared to the time spent trying to use 3D toolpaths.

In the attached file are a few different toolpaths supplied as examples for you to study, also just program one groove and then use the Pattern facility in Manufacture to do all the grooves. Lots of ways to do it, these would be the easiest to me.

[Muzzerboy]

Thanks for the thoughts there. Note that I only plan to make one instance of this part.

What confused me is how Fusion knows to follow the sketch path you created at the base of the slot, even though the control point on the cutter is at the base of the cutter ie in line with the "lower" wall of the finished slot and offset 0.9mm. It seems to be clever enough to figure out what is needed when you help it, yet can't do so when pointed at any of the actual features of the slot. Having to create sketch lines to help it out (and indeed knowing when you have to) seems like "fiddling" to me. It's particularly galling when the 3D Contour manages it without any messing about at all - click on the profile and you are done - if only the lead-in and lead-out were controllable...

I have 1.8mm ball end mills that would do this job directly but the cutting speed at the centre of a ball end mill tool is zero, so you end up with a messy surface finish and there are 32 of these slots per pulley (and 16 in its friend, FWIW), so a lot of slot length to cut. Beyond getting her done, I am also aware that I will likely come across something similar in the future, so understanding the options and how to configure them feels like a good investment - within reason of course. For which, thanks for your input!

The tool I modelled is a catalog part - actually a Korloy NFTIH boring tool with a 1.8mm diameter contour insert. The insert is within 0.01mm of the required radius, so good enough for the application (timing belt pulley).

The corner radii at the top of the slot are supposed to be 0.3mm but I'll simply use a std 0.5mm cutter. Again, we have to keep in mind what this is for.

By the time I'd made up a custom cutter I'd have spent more time and money on the cutter than the part, even if I had the means to make it to any degree of accuracy, which I don't.

I am familiar with circular pattern but posted a simple model here to avoid uploading my entire assembly. I certainly wasn't planning on running 32 instances of the program...

[mailRQAJW]

@Muzzerboy 

Well, if it was me doing this (Of course it isn`t) and it was a "one off" pair then I would just buy a set of pulleys and a belt from a gear manufacturer, done it often over the years, if doing a "Custom" groove length with a length turned down that wasn`t standard then again I would get the people that have the machinery to do it quick and clean, including any keyways, bores required at a price that would be well below the hourly rate I have to live with in the shop, in the time taken to make the pulleys myself I could make a lot more from Customers jobs!!

Another way I have done what you are doing is to just buy a couple of lengths of "Toothed Bar" the right length/diameter/# grooves and turn down where I wanted it round in the Lathe

If it is just a Project and you are not bothered about the cost of the time spent then great, it is always nice to work something out and make a part from scratch, very satisfying, what is the saying? "Every day is a School Day"

Good luck with it.