Depth cuts & steps by depth?

[William Grizwald]

Ok, another simple thing I'm sure...

 

I'm contour milling 2 long parallel paths - up one side, down the other. If I select Depth Cuts/ By Depth, the tool alternates back and forth between each path efficiently. But, when I add Multi-passes to the mix, it defaults to wanting to rapid all the way back to the start to complete that paths stepover first before moving to the next contour. What's the trick to combine both and be efficient?

 

Thanks,

 

--

Bill

[Thad]

It could be a limitation to multipass, I'm not sure.

 

Maybe you could connect the two lines with a dummy line. Then use change at point to make it a rapid stepover.

 

OR

 

If you need (for example) a single multipass of 1", program it to leave 1" stock, then copy the ops and change your stock to leave to zero (or whatever). Post all ops together and you're all set. Kind of a poor man's multipass.

 

Thad

[Lee.]

Bill,

 

I've done what Thad talked secondly about before, when it's just too time consuming to rough/pocket.

 

Good Luck.

[William Grizwald]

Thad & Lee,

 

I've been creating a pseudo line between the paths to make it work in the past. The problem there is then the tool has to extend past the part far enough for the tool not to rapid across the side of the part (depending on the ammount of stepover). For this example, it means the tool must feed past the part 8" min before it can rapid across (not real efficient). The part is 22' long so I'm always looking for a shorter path...

 

The other option of creating yet more operations (or transforms) is REALLY not my first choice as most programs seem to be 100+ operations. I need to step down 3 levels to finish. But, for the sake of efficient code, it appears to be best option for now.

 

 

Thanks guys.

--

Bill

[Troy Gossett Indepak Inc.]

I'm with William here this should work the way he explains it. Work arounds are for software that doesn't work right in the first place.

[MLS]

Offset your geomtry the multipass width you want to make a copy then select the additional chains with the originals in the order you want them to cut. (with multi-pass off)

 

 

My solution if connecting the ends won't do.

 

I have often wished we had more control over this in fact.

[Lee.]

William,

 

if you like send me the part with an explanation of what you want to do.

 

I'll take alook at it.

 

Lee.

[Guest]

If I understand you correctly, you are not maintaining cut direction, climb/conventional, what you want to do is doable but YOU will need to create geometry to do it.

[Troy Gossett Indepak Inc.]

I've also extended the lines and closed them to make a pocket path constant overlap, in to out. This still is more work than it should be. Multi pass should have by contour like depth cuts has by depth option.

[William Grizwald]

John, all,

 

Imagine a machining a section of railroad track. I'm driving the tool along X- , rapid across Y drive back along X+.

 

I need to step down and step over on each rail because the rails are wide and because of extra stock. I don't want to rapid all the way back to the start of each rail, I prefer to "racetrack" the path if you get my drift.

 

Pretty simple stuff really. I can't imagine not being able to go this in one operation... does this make sense now?

 

--

Bill

[MLS]

William,

 

You are going to have to create the extra chains(offset) instead of using Multipass. Then select them in the order you want to cut them.

 

------------>

geometry now

<------------

 

 

------------>

------------>

geometry you need

<-----------

<-----------

[Jack Neelands™]

create an arc on each end the size of the slot...

then translate them out (1X the dia) and trim the lines to the arcs

Ramp the cutter down using multipass and make sure your start point is midpoint of arc as the start of toolpath

[William Grizwald]

Ok so MLS had the best answer for my problem...

 

Btw, Lee you have mail (Jay's ftp didn't connect), but I think this is the best fix.

 

I created the additional step over geometry lines then selected them in the proper cutting order. I Then applied depth cuts which stepped down after completing the initial stepovers.

 

You all have to understand (coming from another system) I'm not used to creating a lot of extra geometry for nc toolpath unless it's complex surfacing... That said, the workaround - works.

 

--

Bill

[MLS]

William

 

I totally agree.

 

It IS a workaround IMO.

 

I would prefer the ability to control the order of multi-pass AND depth cuts in all possible scenarios as well.

 

Glad you got it to work though.

[Thad]

William,

 

I suggest you submit this to [email protected]. If it's a bug, they should fix it. If it's not a bug, they should log it as an enhancement request.

 

Thad

[William Grizwald]

Thad,

 

It's not a bug. There is no "switch" in Multi-passes for depth or contour like Depthcuts. As part of my job, I do document these types of things. I wait though to make sure there is not a method that is already there that I'm just overlooking.

 

Btw, the immediate weakness of my fix became appearent when I just had to replace the 4" facemill with a 5"...

 

--

Bill

[Rick Henrickson 65]

what about surface rough contour, or hsm tool path core roughing ?

[Steve Arteman]

Bill,

Have you tried to use Ramp by depthin contour? chain single one side and then the other in the direction you want to cut, excellent for rib cutting a single chain in both directions and include both chains.

Check it out

Steve

[Thad]

quote:

---

It's not a bug.

---

quote:

---

If it's not a bug, they should log it as an enhancement request.

---

Either way, I'd let CNC Software decide if it's a bug or not. Things that go unreported don't get fixed/changed and then people continue to bitch about them because it still doesn't work. For the record, I'm not saying you're bitching but I think others are. There's nothing wrong with that, but now's the time to do something about it.

 

Thad

[Guest]

When thinking about cutting as you describe it goes right to the heart of maintaining cut direction and cutter comp. I am guessing this does not work that way without creating geometry because it goes completely against this principle.

 

The only thing I think you'll be able to do is create your zig-zag at the proper steps for your cutter size and use a contour will cutter comp off, then it will follow the line.

 

Otherwise your into automatic toolpath creation and it WILL try to maintain cut direction.

[MLS]

William,

 

If you create the Geometry centerline, changing tools is an enormous weakness, but I would suggest creating the geometry relative to the model and still driving it with comp. This will allow you to change only the cutter and REGEN the toolpath.

 

I am so used to creating geometry, I never think twice about it.

 

The way multipass/depth cuts on contour toolpath works now is perfect for melting down a contour, I just wish we had the control to melt OUT a contour so it takes all the depth cuts prior to making a radial offset.

[William Grizwald]

MLS,

 

I created the geometry as a profile to drive the tool using Comp/Computer. Works ok. I just had to offset the lines to respect the increased stepover.

 

No biggie. Thanks!

 

--

Bill

[MLS]