3D machining profile, Boundary Taper negative value.

[dkemppai]

Hi,

So, it seems that using a boundary shape ID allows one to trim a 3D machining operation to a boundary shape. The boundary taper seem to work well also, however taper gives positive results only (Making the boundary taper wider at the top.

I have an application where I'd like a negative boundary taper. That is, Narrower at the top than the bottom, for an outside machining operation. It would be nice if the boundary taper allowed both negative and positive values to tip the boundary in or out as needed.

The application is 3D profile on the end of a round bar. I've removed most of the extra stock with the lathe, and would like to tip the boundary to be smaller at the top. This would allow much less cutting of 'air'.

Thanks,
Dan

[Bob La Londe]

You can always create a (-) offset from your Shape ID used to create your boundary, and then use that as the Boundary shape. 

[dkemppai]

Hi Bob,

OK, maybe there is a technique i'm missing, so if you have time to show me, by all means... 

Anyway this is the object I'm trying to create. I start with a bar, and turn some of the rough stock off, leaving what's in red (transparent so you can see the target design underneath...)

Then I use a 3D rough profile to hog out the rest of the metal, and then follow with a finish pass.

You can see there is a boundary profile object (circle, 14), that sets the boundary with a boundary margin to force cutting out to the edge of the boundary. However since I have a tapered stock to start with, I don't want to mill air where metal is already removed. Setting the boundary taper setting of both positive and negative both swell the tool paths larger at the top. (CB screen shot). One would expect negative to shrink it and positive expanded it, or vise versa (As with many other settings in cambam).

See attached images, and .cb file...

Merry Christmas!

Dan

[Bob La Londe]

I think I might have heard the wrong question.  Try setting a depth of increment zero for finish passes in horizontal or vertical, or set waterline finish instead of waterline rough if you want to waterline the part. 

Nobody wants to cut air.  Well except maybe at a Texas Chili Cook Off. 

[Bob La Londe]

Ok...  I'm not sure what you are trying to accomplish, but I do not see how that taper is necessary at all.  

Just circle the stock with a shape one tool diameter larger (or more if you want less than 50% engagement of the tool) than the rod stock and use selected shape as you did.  Screw the taper.  Its not needed.  

Its going to stop at whatever depth you selected.  So there is no need to use a bounding circle the exact size of the part.  

Your second MOP works fine without the selected shape.

[dkemppai]

Hi Bob,

OK, maybe I'm not being clear. See image. I want to turn the object on the left into the object on the right, but not waste time cutting a lot of air.  I did not use boundary taper for my actual rough, because it didn't work like I wanted it to. I wanted to use it to save cycle time, where A LOT of air was being cut. Make sense?

The part is relatively hard 1050 steel, I didn't want to burn cutter life on a small carbide ball end mill. So I removed extra material in the lathe.  Maybe 40% of the waste volume was removed with a lathe in about 60 seconds...

So, I started with a bar with a tapered end (Left image), then 3D milled the final shape into it (Right image). Because a bunch of the steel had been removed previously, it cut a lot of air. However, roughing still needed to be done as a lot of material remained.

I thought the boundary taper could be used to taper the shape moving up from the boundary. It can do that, very well. The only problem is that it can only taper outwards, not inwards. (Many cambam settings work +/-, if a negative sign is used in the setting, roughing clearance for example...)

Try the cambam file I posted. Set both a positive and negative value for boundary taper. If the roughing boundary taper could have been be set to tip inwards, it would have achieved exactly what I wanted.

The part cut well with both MOP's. However about 50% of the machining time in the 16 minute long roughing operation was cutting air. (But, at least it wasn't cutting waste metal burning carbide life! )

Hopefully this make sense now.

Dan

[Bob La Londe]

I can't make it do what isn't there, but an alternative might be to use several 3D waterline finish MOPs starting with a large roughing clearance and eventually finish with zero roughing clearance.  

P.S.  I've been doing some modestly hard steel (4140HT) the last few days, and high flute count AlTiN coated mills are just blowing me away with how much material they can take at a bite.  My limitation is not the mills, but the rigidity of my machines.  1/2" 6 flute AlTiN Accupro... 48 bucks.  Looks like I just took it out of the tube.  Its done many hours of work in steel the last two days.  I just ran a 1/4" 5 flute in the same stuff at high speeds 8600-13000 rpm and 47 to 95 IPM.  Same results.  And I can run flood.  The AlTiN seems to insulate the carbide from thermal shock. 

[dkemppai]

I can't make it do what isn't there, but an alternative might be to use several 3D waterline finish MOPs starting with a large roughing clearance and eventually finish with zero roughing clearance.  

Well, that's why it's in the feature request feedback forum. Taking out an abs(BoundaryTaper) in the code may all it takes... 

Usually when I post, I learn there's some other trick that I missed. I have some ideas for similar projects again, so I was being hopefull for future projects  

I do have a lot of AlTiN coated stuff, and it's great stuff. However, there aren't any AlTiN coated ball end mills in the home shop right now. So, trying to save on carbide that's here.  Once the feeds and speeds dialed in you can cut all day with one cutter. I run a lot of 440C and CPM154 stainless, and a bit of S7. It seems to hold up really well for that.

There's also a place in Canada that CVD coats carbide. Worked great on some big G10 fiberglass. That stuff eats regular carbide fast, and the coated stuff did the job with one cutter... 
http://www.cvddiamond.com/products

Merry Christmas!

Dan

[EddyCurrent]

I thought about using Edit->Surface->Plane Slice Z with 0.015" slices.

There are problems though;
1. Unless one or two 'Roughing Clearance' passes can be used, the tool is taking a full depth bite.
2. If using a Profile MOp with each polyline the Z depth would have to be entered for each one.
3. I thought about using Edit->Offset (by tool radius) then using an Engrave MOp so that Z would be taken care of.
It turns out though that the resulting offset polyline sets Z to zero.
I might add a new offset plugin or script that retains the Z value but it could only work if the polyline was flat in Z.

[EddyCurrent]

I've attached a cb file with some of the Profile MOps entered to see what it looks like.
I think it's easier to let it cut some air 

[Bob La Londe]

I can't make it do what isn't there, but an alternative might be to use several 3D waterline finish MOPs starting with a large roughing clearance and eventually finish with zero roughing clearance.  

Well, that's why it's in the feature request feedback forum. Taking out an abs(BoundaryTaper) in the code may all it takes... 

My mistake.  I made the apparently false assumption that you might appreciate another way to get more efficient code than you are using.  Won't happen again.  My apologies. 

I've attached a cb file with some of the Profile MOps entered to see what it looks like.
I think it's easier to let it cut some air 

For one off custom parts IT IS OFTEN FASTER (net time) to just let it cut air or use less efficient code, but as soon as you have to make a second or third identical part its time to give the efficiency of your code a hard look. 

[EddyCurrent]

Bob,  I don't think you made a mistake when Dan said this, but if you did then I also followed on with the same mistake.

Hi Bob,

OK, maybe there is a technique i'm missing, so if you have time to show me, by all means... 

[dkemppai]

Ok, First, please do not take offence. None is intended here. Sorry if I did so.

Bob, you have offered help many times in the past, so I do appreciate your input. Very much. However, your comment about not making it do something that isn't there seemed a bit sharp. Sorry if I snapped back.

I agree letting it cut air is faster for a one off. However the engineer in me always wonders if there's a better way. So, when I spotted the boundary and boundary taper options, and I absolutely knew they would do what I needed. Placed the boundary circle, and set the taper...   ...then set the taper negative. Both made it larger. Hmmm, that's weird, time for feature request.

Usually when I post there's a clever way to do something I haven't thought of yet. Maybe defining the stock with a 3D object, or some other neat little trick. Dunno, you guys are darned good at this.

Sorry to drag you into this problem.

Thanks,
Dan

[EddyCurrent]

Earlier I said this;
"I might add a new offset plugin or script that retains the Z value but it could only work if the polyline was flat in Z."

So that's done now and it's here; http://www.cambam.co.uk/forum/index.php?topic=7052.msg57426#msg57426

[Bubba]

Thank you Eddy.

 Merry Christmas to All who celebrate!