How do I hold it

[Rickg5106]

Hello All,

Trying to change the angle on the exhaust cans on a motorcycle.  Solution is to cut some "Wedges" that will be inserted between the pipe and the can.

First setup will be in a vice to face and get the center and bolt holes.

Second will be a fixture holding the center hole and locating with the bolt holes to cut the profile.

The third setup will require a compound angle facing and a gasket slot at an angle yet to be determined.  The last operation will be done in mirrored pairs. 

Not sure how to hold for the last operation. Something REASONABLY robust will be warranted as I'm not sure how many of these things I am going to have to make. Maybe 1, maybe 1000.

 

Attached please find a screen dump of the part. Dimensions are for reference as we have not finalized the design, (waiting customer input).

Thanks in advance,

Rick 

[Guest]

Hold it in a vise as stated

 

Cut the top angled face, then use a slitting saw to cut it off complete

[mkd]

assuming you are limited to 3 axis, it sounds like you need to figure a way to prop up your vise in order to machine some soft jaws.

- or prop up your jaws in the vise.

[jlw™]

I've got two of these:

 

http://www.ebay.com/itm/like/321340977520?ul_noapp=true&ul_ref=http%253A%252F%252Frover.ebay.com%252Frover%252F1%252F711-117182-37290-0%252F2%253Fmtid%253D1588%2526kwid%253D1%2526crlp%253D53601919689_324272%2526itemid%253D321340977520%2526targetid%253D154774693929%2526rpc%253D0.14%2526rpc_upld_id%253D63956%2526device%253Dm%2526mpre%253Dhttp%25253A%25252F%25252Fwww.ebay.com%25252Fulk%25252Fitm%25252Flike%25252F321340977520%25253Flpid%25253D82%252526chn%25253Dps%2526adtype%253Dpla%2526googleloc%253D1013042%2526poi%253D%2526campaignid%253D239125209%2526adgroupid%253D14978428809%2526rlsatarget%253Dpla-154774693929%2526gclid%253DCIKrrMf1mssCFQ8kgQodS4kOQQ%2526srcrot%253D711-117182-37290-0%2526rvr_id%253D989199491993&chn=ps&lpid=82

 

in my play shop and we have a few bigger ones at work. They work really well if you don't try to hog on it. I always give an MDI program to indicate the angle.

[#Rekd™]

I would do the the side with the counter bore first, only the hole, the counter bore and the clear holes while holding it in a vise using 5/8 thick material and the length and width enough for some clamps or holes when you flip it. Then I would make a jig to flip the part over and locate the bore and 2 of the clear holes, clamp or screw it to the jig. Then surface the angular face, then cookie cutter the outside leaving about 0.01" to 0.02" at the bottom (not sure what material you are using). Then snap the outside parts off and file to clean up.

[Newbeeee™]

I'd do the flat c/bore side first:- profile the outside, drill 4x holes, c/bore, and not so the bore - just put a bolt hole through the centre

Flip and sit on a scrap piece of ally with a couple of pins locating in the peripheral drilled holes. Clamp through the centre bore, and scan the angled face (scanning around the cap head in the centre).

Add toolmakers clamps one each side holding the flange, and spiral the centre bore out (with the cap head still in)

[Bob W.]

I would start with stock that is +.275" on the thickness, do the counterbored face first and I would machine all features on that side (center cole, step, profile, and four mount holes).  Then flip it over into aluminum soft jaws, face off the .275" excess, and surface finish the angle using parallel surface finish toolpath.  If an order comes back for 1000 of these I would make 3-4 dedicated, palletized fixtures that could be swapped out in seconds and where the angle is set and no surfacing would be required.

[Bob W.]

Start to finish I'd say a project like this would take 60-90 minutes (if I did everything) or so including programming, setup, machining, and deburring.  Any thoughts?

[jlw™]

I was thinking about the same, most of it due to legwork and setup. Maybe 20 minutes actual run time. And a nice clean angle like that I'd 3d with a 3/4in bull mill.

[#Rekd™]

My guess based on our equipment and tooling would be 3 hours. Fully finished part and machine is cleaned.

 

There is one guy in my shop that would spend 8 hours programming it and running! He sets the external off set in the Z above the part and dry runs the entire program...enough said!!!

[Bob W.]

There is one guy in my shop that would spend 8 hours programming it and running! He sets the external off set in the Z above the part and dry runs the entire program...enough said!!!

That's why some guys make $35/hr and some make $20/hr.  If he were to use the tools at his disposal correctly there is no need to dry run.  We never dry run and I always expect the first part to come off the machine good.  We don't bank on the first part being scrap ever.  We use the overlay in verify to check programming errors or oversights and if there are tight tolerances the tool wear is set to zero so that dimension can be crept up on. 

[taperlength]

I'd get it plasma cut. The bore is not a cosmetic feature, so hold it there, face, finish the outside and drill the holes.  Then flip it over onto an angle fixture and finish the other side.

[#Rekd™]

That's why some guys make $35/hr and some make $20/hr.  If he were to use the tools at his disposal correctly there is no need to dry run.  We never dry run and I always expect the first part to come off the machine good.  We don't bank on the first part being scrap ever.  We use the overlay in verify to check programming errors or oversights and if there are tight tolerances the tool wear is set to zero so that dimension can be crept up on. 

I agree 100% Bob, I am talking about a guy that makes a cad drawing to make a math calculation!

 

The same guy changed a set of bearings in an electrical motor (about 3/4hp) took him 3 hours, I did the exact same make and size of motor the next week in 35 minutes.

 

Sorry to hi-jack this thread!!

[jmfrank]

What material will these be made of ?

[crazy^millman]

What material will these be made of ?

 

Was wondering when someone was going to ask that question. You guys got it all figured out without knowing what the material to be cut was. I was on Vacation and I looked at this and that is always my 1st question. What is the Material we are cutting? What is the size of the Material and what machine are we cutting it on? Do you have specific tool(s)/brand(s) you want us to use or can we pick what we think is best? Then many other questions from that point forward.

 

1 off or 1000 is totally different concept and approach and see to many people fall for the carrot. Quote them to make 1 part. Then quote them to make 1000 parts. I hate that well give us a quote based off of getting 1000 parts. It is the classic bait and switch. Sorry we have a business to run and we will quote you based off of what it takes. Then you can decide if you want to work with us or not. 

 

Side note we did work for Yoshimura a couple years back and I think they already make something like this. Might get on their website and see how much they are charging for theirs.

[ScottBro4]

I have done parts pretty similar to this.There is a pretty simple but somewhat pain of a way to done this accurately. Finish thru hole from one side, face, drill and tap bolt holes. Make fixture to hold the part down with bolts and locate off ID features. Cut profile and surface the other face on angle. Then, without removing from the fixture, cap over the ID and drill the tapped holes out. Good luck.

[betts]

I'm with Ron, I need to know the material.  I was waiting to hear what it was mostly because I had a possible design concern.  Going from over 1/2" down to .034 on that corner with the hole thru it, I hope material choice was given some thought.  With the heat/cool cycles of exhaust you wouldn't want to have failure issues.

[Newbeeee™]

True Ron.

I'd assumed it's ally because I've made a few similar things back in the day and ally is fine for tail cans.

Also ref my method, I'd assumed onesey twoseys because you're not going to make a 1000 without first making the prototypes. For qty I'd go with chick jaws as Bob said.

[Bob W.]

I figured the material would be steel but whether it was steel, stainless, or aluminum it wouldn't change my approach for 1-2 pieces.

[Thee Dragracer1951]

I'd cut the side normal to the bores first .  put it in soft jaws and surface the back side with a good sized bull endmill.  maybe an.06 rad.  

Whole deal done in about an hour.  Or like Bob said,  maybe a little longer. 

easy job.

[crazy^millman]

I figured the material would be steel but whether it was steel, stainless, or aluminum it wouldn't change my approach for 1-2 pieces.

 

It wasn't meant to be negative and why I stayed out of the thread until the question was asked. I guess all the crazy parts I have had to cut and all the well BTW we would like this out of wasp alloy or Inconel 718 at the same price you quoted that 6061 aluminum part at have me thinking out loud.

[SpacePilotPro]

Hold it in a vise as stated

 

Cut the top angled face, then use a slitting saw to cut it off complete

 

I agree totally with this method if it is aluminum.

[ScottBro4]

Regardless of material, with the right feeds and speeds this part will not bow that much. Unless this is for a customer and there is a flatness call out I personally wouldn't be worried. In the end it will be sandwiched between 2 flanges and that will pull it flat. Just my opinion and experience with parts like this. 

[Rickg5106]

Sorry for the late reply all, had to get my knee scoped and have been off the 'puter for a bit.

Material is 6061, though it will be mating to steel exhaust parts.  It will be right before the exhaust can so combustion heat won't be much of an issue.

The bike manufacturer set the cans so they splay out from the from the tailpiece in the Y and also don't match the seat sub-frame angle in the Z.  Everybody hates the look so these would be used to "correct" the angles.

My thoughts are to make a profiling fixture to do the outside in the second operation, a flat plate with the bolt holes as pins and a bolt down cap to hold the piece with the center hole.

For the third OP, make another fixture to cut the the compound face with the angle set and pins to orient for the compound angle on the piece. I though about locating with three bolt holes that would remain "fat" and using the gas hole for some kind of hold down strategy that would be below finished surface.

I sort of dreamed up some kind of sharp edged eccentric that would bite into the gas hole but didn't think that would be robust enough. Flying parts are never a good thing!

But sometimes I tend to make things complicated and wonderful so I was hoping for a better thought.

[greenxman]

I would sub it to one of these guys and charge double. in the end its all about the all mighty  $