Mandrel bend cutting jig

I've now got myself a load of 32mm mandrel bends in 45 degree and 90 degree segments. However, I'll need to chop some of them off at other angles. They could be pretty tricky to hold while using a bandsaw or angle grinder to cut them to the required angle.

There are a few examples of 3D models that achieve this function on places like Thingiverse etc. Naively, I thought I might be able to download something that I could simply print out and use - something like these:

...but the only models I could find were expecting some form of payment, either as STL files or even as the printed items themselves, with prices ranging from ~£5 (model) to £40 (printed). Well fuck that. Apart from that being against my religion, many of them don't actually do what I need, not least being for the wrong diameter tube and none of them are parametric or even in Fusion format. Details, I know.

Fusion time:

What I want:

• Suitable for 32mm tube (ie OD, not ID)
• Settable at 5 degree increments
• Split halves, to allow easy setting and clamping
• 1mm gap between the halves so there's movement for the vise to clamp the tube
• 10mm dowels to hold halves together before being clamped
• Solid (100%) fill in ABS, so it can be solidly clamped

Like this perhaps:

Obvs you need to account for the diameter of the stop pin when setting the angular positions of the holes. Like this:

Lots of support structures in the various holes. This is my first trial attempt, using default settings (to save material). 

Came out OK but made a couple of enhancements to the design, namely:

• Rather than use 10mm dowels to align the halves, use M10 screws with captive nuts, so I can nip them up before going into the bandsaw vise.
• Use an M4 caphead screw for the tube stop. And provide a counterbore for the head on the reverse side - or in fact a whole series of them, one for each position.
• Reduce the gap between the halves from 1mm to 0.1mm. Yes, it still clamps nicely but doesn't wobble around.
• Use 100% fill, as I'm reasonably confident this is in a good enough state not to require further iterations.

And it finally printed out after 7.5 hours. Using the default fill of 25%(?) would have only saved me about 30 minutes apparently. The main difference of going for 100% fill is the cost of the material. Total usage should be around 187g. At about £15 per kg, that's about £2.85 for the final part ie not exactly extravagant.

But after some poking and pulling, it's all cleared out and working. Reamed out the holes with a couple of drills and it's a good 'un.

I will need to cut that M4 screw down to 45mm so it doesn't poke out. Later.

Also, the big M10 screws holding the halves together need to be 45mm long. Seems I have only one M10 caphead screw in my entire collection and it's about 60mm long. That's a great excuse to buy some 30, 45 and 60mm for my "stock". I'm not ready to do any pipe cutting and welding yet, so completing the final assembly of this thing can wait until I have the final delivery of u-bends from China and the screws from ebay.

Job done.

Modelling a bunch of bananas - aka downstream manifold

Modelling? Bananas?

There seem to be 2 ways to go about fabricating an exhaust system, particularly the manifold end, where things tend to be more complex: the Honda S800 has a "bunch of bananas" manifold, forming a 4-into-2 system with equal length headers.

The first method is simply to get a pile of tubes, elbow bends, angle grinder disks, welding wire etc and knock it up piece by piece. 

The second is to model up the system using standardised building blocks comprising mandrel bends and sections of standard tubing. Unless you intend to persist with the use of tube benders, you have little choice. Even then, the tube diameter and bend radius are all going to be fairly well predefined. And given that the 32mm tube I have seems to collapse when you so much as fart next to it when trying to bend it more than 30 degrees or so, my attentions have focused on the use of mandrel bends and u-bends, chopped up as required, then butt welded together to form the required final assembly.

And when it comes to modelling manifolds in Fusion 360, there are 2 approaches.

1. Make up a library of bends and tubes, then assemble them so that they replicate the real thing. Then replicate each compt on the bench and assemble / weld them up.
2. Create a 3D sketch that defines the centre lines of the headers, then finally use the "pipe" feature in Fusion to create a pipe that follows the sketch line. Alternatively, you could create your own tube section in a sketch and then use the sweep function to create your own tube / pipe. 
   

NB: Interestingly, the "Pipe" tool in Fusion should really be called a "Tube" tool, as the diameter you specify actually ends up being the OD, not the ID: if you specify a 32mm pipe diameter and a 1.5mm wall thickness, the ID measures at 29mm.

The 3D sketch method is a royal PITA but as log as you don't define the dimensions of the angles and length of the subcomponents, you can edit them in place by dragging the end points of the sketch segments in the 3D environment - assuming you have selected "3D sketch" in he sketch popup dialogue. In contrast, the "build it from blocks" approach is a different kind of royal PITA - each time you want to move the parts around, you have to either use revolute joints etc (for rotation) or edit the subcomponents for each position, noting that you will need to unlink them from the original, to avoid changing all instances at once. So you will end up with a myriad different tubes and elbows and moving each about will be the devil's work.

Here's an example of how to use the 3D sketch method. It's got no commentary but even so, you can see that it's not dead simple:

And LEAD has a similar video in that wonderfully condescending fashion so many Mercan Youtube heroes adapt.

Enough talk - time for some action:

Here's the beginning of an assembly using the "building block" method:

I soon gave up on this, as it was clearly going to become a nightmare very quickly.

Here's the "3D sketch" method, with the centre line sketch being open and edited. The blue lines are not fully constrained, so can often (sometimes?) be edited by dragging the segment end points.

If you set the sketch properties to "Show dimensions" and keep the sketches visible, you can also see the dimensions (look closely):

Changing the Display Settings / Visual Style to "Shaded with visible edges only", highlights where the different segments abut:

And of course, you can render it if you are a CAD tart. The stainless tube I bought is actually polished (it was actually cheaper than the "natural" finish), so it's actually quite close to what we might expect to see, apart from the heat discolouration.

I've concluded that the 2 lower headers may as well join before the final exit (as shown), as this would simplify the assembly and I don't imagine shortening 2 of the headers by a couple of inches will make the slightest difference. That will require some further CAD work of course and the tube is slightly larger diameter (38mm) after the 2 headers merge.

WTF is wrong with Fusion toolpath simulation - takes forever - SIMPLE FIX!

Dunno what is wrong with my PC. It takes almost forever to simulate the toolpath for the exhaust flange. It's not a large or complex part but I timed it consistently at 5:30 minutes to complete a simulation.

That simulation is the generation of the toolpath and, in particular, the stock removal. There are quite a few contributors to the processing time:

• I don't have a particularly powerful processor in my PC. It's a GMKTEK NUCBOX9 (SFF tiny PC thing) with an AMD Ryzen 5 5600U. This is considered to be broadly equivalent to an Intel Core i5-1135G7. It should be fine for my needs - and better than the previous PC I was running - which in turn seemed to be well powerful enough.
• It has an inbuilt Radeon Vega 7 integrated graphics, which is generally thought to be good enough to play "light and casual" games. I'm only running fairly simple CAD graphics here - and Fusion isn't that demanding when it comes to graphics. Gone are the days when you had to run a Quadra (CAD) or a high end gaming graphics board.
• I'm running 3 displays at 1080p aka FHD. That's not quite 2K and certainly not 4K resolution but it's fine for my needs and my monitors can't do better. The Radeon graphics should be fine with that.
• I have plenty of RAM now, having upgraded to 64GB. With Fusion running with 16GB, I was running out of working RAM, with the risk of having to use the swap file which slows stuff down a fair bit.
• It seems to be the adaptive toolpaths that really hammer the simulation times. Sure enough, the adaptive part of the operation dominates the time by far:
• Adaptive 2:55
• Bore 1:05
• 2D Contour 0:33
• Drill 0:07 (hard to time it precisely though)

But waiting for over 5 minutes to get a toolpath simulation completed is taking the piss. Some thing needs to be done - and it won't involve buying a more powerful PC.

In the interests of science - and to avoid losing the will to live during toolpath simulation, I tried changing various settings:

• Unselecting the various "Display Graphics Effects" options that are set by default:
• Ground plane
• Ground shadow
• Ground reflection
• Object shadow
• Anti aliasing

These made sod all difference.

• Then I messed with the settings within the adaptive toolpath, namely the tolerance and the fine stepdown, which seems to be set to 10% of the roughing stepdown by default. I increased it to 1mm.

That did f*ck all too, so I put it back to 0.3mm.

• Finally, I reduced the "Accuracy" setting in the Stock section of the simulation dialogue box. The slider has 10 positions and is set to 10 by default. Position #1 is "minimum accuracy" and #10 is "max accuracy".

This utterly transformed the performance - setting to mid position (#5) removes the bottle neck. Running just the Adaptive toolpath, we now get ~00:26, down from almost 3 minutes.

• You can then increase the speed of the displayed simulation without being held back by the processor trying to keep up. In fact, it can generate run the whole toolpath within ~3 seconds and it's the graphics that struggles to display the toolpath, not the processor doing the calculations. But what is the sweet spot? How much can I turn the "accuracy" slider back up before affecting the simulation time?
• Interestingly, when you change the slider position, a text appears, saying the stock generation is being completed. It seems to recalculate the stock automatically each time a change is made to the accuracy slider setting. As this stock generation seems to be the cause of the issue, we can simply focus on those times, rather than run the whole simulation each time. And here's what I found for the stock generation time for each slider setting:
• #5 < 1second
• #6 ~3 seconds
• #7 ~3 seconds
• #8 ~4 seconds
• #9 ~35 seconds
• #10 1:44 minutes.

Here's the "stock generation" text, visible at the bottom of the screen if you look closely:

These times are fairly approximate because it's actually quite difficult to measure without some sort of anal video capture approach. I have a life to live, so that isn't going to be how I do this. I just used the stopwatch on my phone.

But there we have it. Simply putting the accuracy slider to position #8 largely sorts the problem out. I'll leave it set to #7, at which point, the only bottle neck seen occurs if you crank up the simulation display speed to something dumb, where the graphics struggles to display enough FPS to give a smooth view.

So indeed there we have it. The fix is actually very simple. That feels like a result.

Machining the flange - cockup central

Here's the toolpath in Fusion CAM. Fatboy here fancies using the 8mm end mill to drill out the 9mm bores for the fixing bolts. More sensible punters would opt for a 9mm drill. More about this later...

In the CNC12 controls, the gcode is loaded and ready to go.

That seems to be going OK, although the ramp feedrate is abysmally slow. Can't be arsed to rerun the toolpaths, though.

It doesn't sound happy with the grievously slow ramp. It's in danger of rubbing rather than cutting - the last thing you want when machining stainless steel, since this is liable to cause work hardening. You really need to go big or go home but yesterday I wimped out and cut the feeds and speeds by the best part of 50%. Furthermore, cutting a slot using a profile toolpath with 100% optimal(?) load possibly isn't clever. An adaptive toolpath might have been a bit more obvious and sensible.

But it seems to be coping ok so far....

By this point, the bores and bolt holes are done. The bolt holes were probably a stupid thing to do - using an 8mm end mill to bore a 9mm hole leaves very little room for chip evacuation. After the first couple of holes, the swarf changed from nice clean ribbons to something more like filings. I think I had damaged the tool before finishing those bolt holes.

Next (last) is the profile operation. This should ramp down progressively as the tool runs around the outer profile. The stepdown was a rather girlie 2.6mm per pass. That's barely using the tool - and I've almost certainly buggered the tool by this stage.

On the second pass, by which time tool was cutting at its "full" depth of 2.6mm, there was a loud click and a change in the sound of the tool cutting. And instead of cutting chips, it was trying its hand at stir welding.

So that's the end of that (rather expensive) tool. On the upside, the machined bores are a nice fit to the tube. 

So without further CNC carnage, I'll simply flash up the bandsaw and liberate the flange.

With some angle grinder and belt sander action, I've recovered the flange from the stock.

That doesn't look too bad, although perhaps 7-8mm thick stock would have been a better choice.

The 32mm tube is a nice snug fit.

Looks like a reasonable result if you overlook the fucked up end mill.

CAM setup for the flange plate

I have a couple of these end mills from SGS Tool (now branded as Kyocera SGS). Called "V-Carb 55SS Short", aka "Series 55":

They are recommended for steels, stainless steels, cast iron and high temp alloys, so should be good for my 304 stainless flange. And furthermore, they both appear to be in decent condition ie not buggered or chipped.

The reason for looking them up is to get the recommended cutting feeds and speeds:

For profile cutting with an 8mm cutter (2nd column), it looks like 3090rpm; for HSM (adaptive), 4665rpm and feed rate 26um per tooth (profile); 51um per tooth (HSM).

Double check that I understand correctly:

• 51um feed per tooth for 5 flute cutter at 4665rpm >> 1194 mm/min
• 26um feed per tooth for 5 flute cutter at 3090rpm >> 396 mm/min

Yes, that computes correctly. 

I don't understand this bit:

Ah:

So it means "keep Ap below 12mm for profile and 16mm for HSM" and "keep Ae below 2mm for profile and 0.4mm for HSM". It's difficult to see how I could keep Ae below 8mm when machining a slot. I guess this means that it's only intended for finishing, not roughing. Ooof yes:

So, possibly not the ideal choice here. What else have I got? I have some V7 INOX cutters from YG in 8mm with 0.5mm nose radius and necked shank with flat (Weldon) shank, p/n EME32906-1. Those are a bit exotic for this application but at least they are rated "excellent" for stainless steels including 300 series.

The data wasn't easy to find but it's held on a Hungarian YG site.

Here's the feeds and speeds table:

For 300 series SS, they recommend 3820rpm, 435 mm/min, Vc = 95 m/min and 28um per tooth. Again, sanity checking gives:

• 3820rpm x 28um x 4 flutes >> 427 mm/min. 
• And the surface speed resulting from 3820rpm and an 8mm cutter >> 96 m/min.

So that all checks out. Finally, for slotting, the depth should not exceed the cutter diameter. But I intend to limit the stepdown to around 2.4mm (30%), as the part will be hanging out over the end of the vice and will only be held on by a few tabs on the last pass.

Looks like a deal. I will dial those numbers back a bit, perhaps 15um per tooth (230 mm/min) and 3000rpm. With some stainless steels, running lower speeds and lighter cuts can cause work hardening but hopefully that won't be an issue here with a fairly modest reduction in F&S.

I'll also have to fill the coolant system again. It got a bit smelly, so I emptied and rinsed it out a few months ago.