Constant Overlap Spiral leaving cusps on the floor

[Thad]

I have a lot of problems with cusps being left of the floor of pockets when using button type cutters. We can cut much faster with a .236 radius than we can with the .062 radis. In order for the button cutter to clean up the entire floor of the pocket, I often have to decrease the stepover amount until it practically negates the increased feed rates.

 

Isn't constant overlap spiral supposed to NOT leave any part of the pocket uncut? My 1.5 dia with .236 rad should be able to step over 1" and still leave a flat floor. Instead, I'm stepping over .9, and while it doesn't show a cusp on the floor in verify, it shows up on the part!

 

Is there a way, other than to decrease the stepover, to assure that I will NEVER leave cusps on the floor of a pocket?

 

Thad

[Mike S @ S4A]

what about surface rough pocket or HST area clearance...? (just throwin' it out there...haven't seen the part)

[Thad]

Mike, I only have mill level 1. These are simple rectangular pockets.

 

Thad

[Mgrenier]

Thad,

 

When this happens, I try to use Parallel Spiral, Clean Corners and that does the trick almost every time.

 

Hope that helps.

[Thad]

Martin,

 

I thought about that, but the most recent incident was a cusp along the length of the pocket, i.e. not in a corner. Kinda like stepping over 1" with a 1" cutter. It's going to leave a cusp. The thing is, I'm not stepping over like that.

 

I'll give it a try anyway.

 

Thad

[rdshear]

For a pocket with square corners, wouldn't you need to have your stepover set to a maximum of .726 using the tool you described. Otherwise, in the corner you would get a cusp because the distance at the 45 would be 1.4142 times your stepover. Or am I thinking wrong?

[Thad]

Rick,

 

I'm not sure what you mean by a pocket with square corners. Do you mean square from the floor to the wall? I'm also unclear on where the 45 comes into play.

 

Thad

[rdshear]

I'm sorry, I meant where the walls meet at a 90 to each other. If the cutter followed the path of the wall, it would make a 90 degree movement in the corners on x/y. If you drew a diagonal from the sharp 90 degree corner through the center of your cutter (the 45 I mentioned) it would be greater than your tool radius. That can create a cusp in the "corner" between passes even though the stepover is small enough to create overlap for straight moves.

 

HTH,

 

Rick

[P_Scott]

Thad,

 

What rdshear is referring to is the distance from the center of the cutter to the corner presuming a 90deg. corner (wall to wall) angle, not the angle from the floor to the wall. You could try the Trochoidal looping by clicking on the High Speed spiral & button in the Rgh/Fin parameters page. The only problem with that is it will probably add more time to the toolpath rather than decrease run time. The benefit of trochoidal loops is that the depth of cut can be much greater, usually as much as 2X or 3X cutter dia, depending on the material. With that tool however, increasing depth of cut may not be an option. HTH

 

Wow, I guess I was way late in replying to this one. Sorry for repeating what you just said rdshear.

[rdshear]

No problem...

 

[MotorCityMinion]

Thad, as a general rule of thumb, I use 70% of the effective cutter dia. to generate clean cutter paths on bottom surfaces. I also use large rad inserts for most roughing opps, .156 being my fav for tool life. That 1.50 dia. cutter with .236 rads should work out to be around ... (1.50 -.236 -.236) x .70 = .72 width of cut or 48% step over. Try a smaller rad to bump up the stepover. If your pinned to using that large of a rad, a finish pass in a seperate opp with a smaller step over and slightly higher feedrate may be the way to go to avoid adding to much time to the cycle.

[Thad]

Looks like I've got to go with a smaller stepover. Rick's and Motor City's math comes out the same. What bothers me is it doesn't show up in verify. That's what I've used in the past to make sure I wasn't leaving cusps on the floor.

 

Thanks for all the input guys!

 

Good seeing you around, Peter. Don't be a stranger.

 

Thad

[mcpgmr]

Thad, I had the same problem and it turned out to be more of a tool pressure and machine dynamics problem. I was stepping over .2 with a .500 cutter that had a .015 rad and still had a slight cusp. I copiied the operation and used a different tool (same geometry) to finish and it cleaned up nicely. I'm running these Kenemetal 3 flute .500 e.m.'s at 8000 rpm with a .003 to .005 chip load in aluminum and they remove the material quite well but still have to take a finish pass to get the FFG surface finish that the boss wanrs. I cant say what FFG means here but you might be able to figure it out.

[Guest CNC Apps Guy 1]

You mean something like this???

 

 

Here's the result when using a .500 tool with a .125 rad stepping over .500...

 

This may be worth adding to the request page.

[Chris Rizzo]

hmmm, I don't see that window in x3, apps guy.

 

 

Thad, what about actually drawing the geo you want the cutter to cut, then run a contour with comp off.

 

kinda ghetto and could be some drawing, but just another idea

[Thad]

Thanks for the suggestion, Chris, but I already do way too much work just to go from what comes out of design to something I can actually cut (efficiently.)

 

Thad

[Guest CNC Apps Guy 1]

It's actually a screen shot from X5 Alpha that I'm sure I'll get in a whole heap of trouble for sharing... j/k it is CATIA's pocket routine... and the radio button I checked and circled will force the software to eliminate the cusps on the floor. It's a nice feature. It shoudl probably be added to the enhancement's topic. I added it here because it was relevant to this conversation, but of course since there is no graphical toolpath editing capability or video documentation it is worthless crap...

[P_Scott]

Thad,

 

quote:

---

Good seeing you around, Peter. Don't be a stranger.

---

Thanks Thad. I won't. I'm still around it's just I actually program much more at my current position and unlike one of the programmers who worked here b4, (not mentioning names in case he's reading/moderating right now, ) I can't spend all day reading and replying to forum posts. I can’t reply as often as I’d like but I do have regular breaks now. B C’ing you.

 

[Thad]

MotorCity, do you use finish pass when pocketing? That seems to be the culprit. I use a good size finish pass so it's more like "just another pass." I only use it to gain the lead in/out on the pocket walls rather than drag up the wall on retract.

 

I used 70% of the cutting dia (as you recommended) and I got a cusp left on the floor. I turned off finish pass and it cuts the entire floor. The cusp isn't in the corner either. It's along the length of the pocket.

 

Thad

[Thad]

Martin,

 

I tried Clean Corners and it worked with a finish pass. I just may have found a winning combination here. Time will tell. Thanks!

 

Thad

[Gary]

So what cnc apps is saying is x3 is basically to releases behind catia? Just putting the wood spoon in the pot for a quick stir

[Guest CNC Apps Guy 1]

Nice one Gary!

 

Actually, I believe CATIA has had this feature for quite some time. For at least the last 2 releases. Flipper could corroborate.

 

:addsalt:

 

:stir:

[MotorCityMinion]

Thad. 6:37 AM. Dedication indeed. I very rarely use the pocketing op., almost always use contour with either a finish pass in the same opp, or I'll dupe the opp and use a fresh cutter. This takes a few more clicks on the calc and messing with the lead in/out options but it seems to produce better results, for me anyways. I've yet to come across a situation where 70% hasn't cleaned up a floor. More often than not though, the number of radial passes set in multipass dictates the step over percentage and I ensure that it doesn't exceed 70%. Bean counters here don't know how to use MC and are not able to calculate the cycle time difference between 58% or 70% step over, but we do piece work here and play it a little safer. Nothing stinks more than pulling a part out of a vise or tearing down a open set-up, seeing a cusp, then having to rerun it with a smaller step over or get out the small stones.

 

[ 08-30-2008, 10:21 AM: Message edited by: MotorCityMinion ]

[MotorCityMinion]

Just thought I'd add this. For verification purposes, you could dupe the opp, use a sharp cornered emill and cut .001 above the floor, the change tool color option in verify SHOULD highlight any high spots, although some times in verify, I have noticed that with walls in particular, setting a rougher to cut at plus .005, then a finisher, (different tool), set at .000 in a separate opp, I,ll see no color change at all and this gets me aggravated quickly as I now have to check all my settings and post code for the tools machining the opp then crunch some numbers to verify that I did indeed leave stock for clean-up. Sometimes I wish I had Vericut, but then again it shouldn't have to be this way in the first place.