Isoline Machining

[Pierre@skeg]

Hi Guys


We are in process of upgrading from 2001 all the way to WF3. Quite something to get used to.


I have what seems to be a stupid problem. When machining rounds on the edge of a block I tried using isoline surfacemachining. The problem is that on some of the rounds the toolpath starts at the top edge and works it way down to the bottom edge of the round and some of the paths it starts from the bottom. This is when machining the round lengthwise as opposed to up and down.


Is there any way I can set the toolpath to always start at the top. Otherwise there is a heavy plunge involved and the first cut is also quite heavy. it is not such a big deal on simple rounds on simple blocks, but when the block gets a bit curvy it gets to be a big deal. I just can't seem to figure out if you can change where the cut starts.I have tried using customize and reversing the toolpath. This just swaps the problem around and the paths that were the right way are now wrong.


I don't want to machine every single round with its own sequence and then customize it, it will take forever. Surely WF3 is smarter than this.


Thanks in advance

 

[appinmi]

If your rounds are continuous, try using the "cutline" definition. The first cutline being the top chain of the rounds, and the second cutline being the bottom chain.


If your rounds go all the way around, select "closed loops" before defining the cutlines.

 

[rocketdude]

Yes That's the answer. I use cutlines nearly all the time in surface machining. Its much more flexible than the isoline dialog.

 

[Pierre@skeg]

Thanks for the reply. We do use cutlines, they just take a couple more mouseclicks to generate. The isoline is a nice and quick way of writing surfaces for rounds and such features. I just thought they had at least gotten round to giving you the option to say from which edge you start machining. It would be a pretty nice toolpath then.


Would you be able to write a UDF that could simulate the isoline machining but with the added flexibility of picking which edge. In other words, use the cutline but reduce the mouseclicks, for simple round machining?

 

[orac]

If your rounds are continuous, try using the "cutline" definition. The first cutline being the top chain of the rounds, and the second cutline being the bottom chain.


If your rounds go all the way around, select "closed loops" before defining the cutlines.

And if you go back to the sequence setup - parameters, you can change the scan type to helical to get one smooth continous toolpath.

John

 

[dibz]

Hi
try 3axis trajectory milling option by selecting all the outer edges of the radius and turning on the "fit to" option.

this gives wonderful results if proper tool selection is done in this case

 

[marker4x4]

Hi

try 3axis trajectory milling option by selecting all the outer edges of the radius and turning on the "fit to" option.



this gives wonderful results if proper tool selection is done in this case

Hi Dibz, could you please elaborate on this technique? I don't think I ever came across that option (fit_to) that you're talking about and it sounds interesting.
Thanks in advance

 

[TonyJager]

Hi Dibz, Marker4x4


I think this technique would work great for cutting fillets where there is a protrusion sticking out of a surface and driving a ball endmill 'around' the protrusion. You would select this option in the customizing of trajectories. When you select edge to drive your tool select fit instead of on/offset. I believe the best way for this to work would be to surpress the fillet around it.


Hope this helps


Tony

 

[dibz]

Hi marker
Tony has explained it already,
but tony , if u delete the radius an do it u can only achieve the radius of the ball nose cutter u r using, and
this is a radius finishing option only,we cant do roughing with this as every one knows