dynamic toolpaths using zig zag cutting method

[wholaday3]

I was wanting to get some feed back on using the zigzag cutting method in the dynamic toolpaths.  I am milling 6061 and using the climb cut method but it cuts a lot of air on the back feed so I tried zigzag to keep the tool in the cut.  I get the same spindle load in both directions but I wanted to know if the tool is wearing faster with zigzag?   Any thoughts would be greatly appreciated.  Thanks.

[mkd]

not in alum.

[daryl_y]

When using  tool path like 2D High Speed Blend I have used zig-zaged in aluminum and have not had any issues.  I have always used climb cutting with the Dynamic tools paths even if these are set to zig-zag they still make a pretty big lead-off and lead-in to you part and seems like there would be a minimal (if any) real time savings.  I doubt you will have any issues aluminum or any other soft material doing this.

[jeff]

I was wanting to get some feed back on using the zig zag cutting method in the dynamic toolpaths.  I am milling 6061 and using the climb cut method but it cuts a lot of air on the back feed so I tried zig zag to keep the tool in the cut.  I get the same spindle load in both directions but I wanted to know if the tool is wearing faster with zig zag?   Any thoughts would be greatly appreciated.  Thanks.

How fast is your machine? I usually set my back feedrate to 1,000ipm. How fast is your rapid?

Personally, I wouldn't be conventional cutting in 6061, you're just asking for trouble. Unless you're trying to finish a steep/thin wall.

[wholaday3]

I use 1000 ipm for the back feedrate on a verticial and 2000 ipm on a horizontal machine.   The parts I have on the horizontal are large so the toolpath seems to spend half the time in a backfeed move to get around the part.  I was testing the zigzag to keep the tool in the cut and it does trim a few minutes out of the cycle time.  Also, I keep the climb and conventional feedrates the same.  Has anyone used the different Motions, Gap size, retracts to cut down on the back feedrate moves?

[jeff]

I use 1000 ipm for the back feedrate on a verticial and 2000 ipm on a horizontal machine.   The parts I have on the horizontal are large so the toolpath seems to spend half the time in a backfeed move to get around the part.  I was testing the zigzag to keep the tool in the cut and it does trim a few minutes out of the cycle time.  Also, I keep the climb and conventional feedrates the same.  Has anyone used the different Motions, Gap size, retracts to cut down on the back feedrate moves?

Ahh, well if the parts are that big, then yeah I can see why you would want to zig zag.  But is trimming a few minutes of cycle time really  worth it?

I can see if you're shaving 30+ minutes, but if it's only 10 minutes on a 1 hour cycle I wouldn't worry about it too much. because setup times can fluctuate that much or more.

 

To cut down on back feedrate moves, maybe you can rough sections of the part at a time? Or quadrants? This might cut down on back/rapid travel time and distance.

[crazy^millman]

What settings have you adjusted in the toolpath for how it processes the cuts? There are 3 options and have you seen what each one does for processing the toolpath? Sometimes you need to think outside the box. Have you tired area rough? Did you make a containment boundary much larger than the part to allow Dynamic to act like area rough? Yes you loose the option to say start from the outside, but if you make the boundary larger when you can in the part then it will mimic area rough where it can and then dynamic where it needs to.

[Roger Peterson]

zig zag works great in aluminum as long as you have tooling and coolant that promote excellent chip evacuation as it will have a greater tendency to load up when conventional milling.  Slowing down the conventional cuts a little can help, but in general I think the gains are minimal and not worth it unless the parts are long, like yours.  I prefer to climb mill and adjust how I program instead.  For example an L shaped pocket, try offsetting the wall geometry to make a smaller pocket just wide enough for your roughing tool to dynamic mill.  Cut the smaller pocket first, then rest machine the larger original pocket.  While not perfect, your tool will spend a lot more time in the cut.

 

 

HTH

[crazy^millman]

zig zag works great in aluminum as long as you have tooling and coolant that promote excellent chip evacuation as it will have a greater tendency to load up when conventional milling.  Slowing down the conventional cuts a little can help, but in general I think the gains are minimal and not worth it unless the parts are long, like yours.  I prefer to climb mill and adjust how I program instead.  For example an L shaped pocket, try offsetting the wall geometry to make a smaller pocket just wide enough for your roughing tool to dynamic mill.  Cut the smaller pocket first, then rest machine the larger original pocket.  While not perfect, your tool will spend a lot more time in the cut.

 

 

HTH

 

Roger I agree and where the cookie cutter just doesn't work sometimes. You need to tear the cookie cutter up and get outside of your comfort zone and just try different things until you nail down something that is doing what you want. I would be against zig-zag for roughing even if it did save some time just because I have seen to much stress added back into parts using that process. By always using high positive tools and climb cutting you pull the stress and heat out of the part. By doing conventional you are adding stress and putting heat back into the part plain and simple. Even a littlebit can make all the difference in the work on some parts. Now for finishing that is a different conversation as the affect zone around the cut acts differently.

[Roger Peterson]

Couldn't agree more, I simply avoid it, not hard to for a thinwall part to curl up like a potato chip.  But to be fair, conventional dynamic milling is still pretty mild compared to the old process' and for some people on some parts it probably has it's place.