Live 5axis programming question

[sharles]

I don't do a lot of true, live 5axis programming. Most of it is 3+2 (locked). The only real multi axis programs I use are drill and curve. But coming up I'm going to be working on  a mold for a 20-quart ice chest and I will need to do the inside and outside of the mold tipped away from the walls for tool clearance. What kind of multi-axis program would I want to look at? I think 10 degrees is plenty of tip, just so the holder clears, especially when I'm inside the mold so I don't hit the part on the opposite wall. Any suggestions would be great!

Thanks,

Scott

[Leon82]

Quite a few of them have settings for tilting for shank and holder clearance.

I've used flow before and tool control from a point  of my choosing for deep features where I wanted the holder to stay in one general area. You can also machine to a point

 

[JohnW@Kauffman]

My go-to paths for the type of cavity work you're talking about are morph and flow.  Both give a number of options for controlling the tool.

[sharles]

are they easy to figure out? I know it took me a little bit to get the hang of multi axis curve...and I should add that was with Ron C'Millman's help...

 

[JohnW@Kauffman]

If you've gotten the hang of 5 ax curve, you'll see some familiar data fields and functions.  Sometimes I have to play around with tool axis control to get the results I want.  Morph will require some wireframe, or surface curves or solid edges to pick "from" and "to" geometry, along with the surface or solid face you want to cut.  I don't do a lot of surface machining, most of my work is trim/drill, but when we cut a mold, I get into the multi axis surface paths on some of them.

[ahaslam]

If you are already familiar with curve, the Morph and Flow are fairly similar. Selecting geometry and tool axis control are primary. I would avoid setting up roughing, linking, and other secondary functions until you have a path that generally flows the way that you want. When first playing around with the paths, set quality and stepover to higher numbers. This helps to allow quicker regen because it may take a few tries.

[ahaslam]

1 minute ago, JohnW@Kauffman said:

If you've gotten the hang of 5 ax curve, you'll see some familiar data fields and functions.  Sometimes I have to play around with tool axis control to get the results I want.  Morph will require some wireframe, or surface curves or solid edges to pick "from" and "to" geometry, along with the surface or solid face you want to cut.  I don't do a lot of surface machining, most of my work is trim/drill, but when we cut a mold, I get into the multi axis surfaces paths on some of them.

Ha, John beat me to it by like 30 seconds.

[JohnW@Kauffman]

One significant difference you'll see in morph is the collision control,  If you've not dealt with that before, it may take you a bit to understand all you can do with it.

[sharles]

I only need to do my finish tools with it. I've got plenty long enough roughing tools to reach as it's only 11.1" tall. Thanks for all your help!

[ahaslam]

Also, Swarf may be a very effective tool path for finishing. I would think using Guide curves with a taper mill and turning on Pattern slices with a forgiving DOC would give a solid path for finishing.

[sharles]

Is collision control like 'collision checking" for the holders in the high speed milling toolpaths?

[ahaslam]

Yes but better because you can trim (avoid if possible), tilt tool (first choice but can be a BZ to get a realistic path) or report errors. Reporting is nice because you can where the issues is and adjust accordingly.

[ahaslam]

In addition, you have two separate checks, one for flutes and one for shake & holder. Turn on number two only if you think the holder will be an issue.

[CJep]

2 hours ago, sharles said:

Is collision control like 'collision checking" for the holders in the high speed milling toolpaths?

In the HSpeed surface finish toolpaths you can also add tilt to avoid a collision. The toolpath will give you simultaneous 5 axis motion without the need for tool axis control geometry. 

[Aaron Eberhard]

Edit:  Whoops, I missed that Chris said this right above.  Good call, Chris.

 

Although of course nothing will replace real training , what you're looking for here is probably to just use a Surface High Speed, probably a Waterline?  On the Holder page, just turn on "tilt to avoid gouge"

After that, you'll get a gouge free toolpath, so for this simple example, it'll start 3 axis:

Then quickly get to 5 axis as it needs clearance:

 

You can, of course, do this with a Parallel toolpath or other multiaxis toolpath, but if you don't really need finite control or don't use it enough to remember what the settings do, why try harder?

High speed tilt away.mcam

[sharles]

ok, it looks like I got waterline to work just fine with a 1.0" ball, but I need to pick it down to a 1/4" ball in the bottom of the cavity and I can't get anything to process...I tried waterline and just limited it to the top of the radius at the bottom and it did nothing. so I tried pencil and it gives me an error...not sure what to do...any suggestions?

[CJep]

Are you using a tool with a taper defined?

The tilt strategy doesn't like tapered shanks, I define them as having a stepped shank then it will produce tilt.

 

[sharles]

yes, my holders are all tapered...even the one that processed fine...but I will go back and change the holder on the smaller tools and see if that's the problem. Thanks for the suggestion...is there a good 'leftover' program in the high speed milling suite? I'm just starting to use them more and so I'm not as familiar with them as I am the legacy toolpaths...

[CJep]

Scott the holder profile is fine, if the tool has a taper defined for the shank that will cause an issue though.

 

Remachining for the HSpeed surface tpaths is now on a page called "stock"

( don't know why they changed the name, kinda like Constantinople / Istanbul ) 

Another possibility for the lack of tilt is not allowing enough of a maximum angle.

 

 

[sharles]

yes, you are correct, my 1.0 ball only needed 10 deg of tip because I could stick it out 4.5" in a Precision Holder 50-1.000-9.0. But my smaller tools needed 15 deg even though I had them in straight shanked, shrink fit holder in the same Precision holder. Just being specific in case any one else is curious.

Thanks a million!