FeatureCAM rapid between open ended cuts while tool is down

Hard to come up with a good title for this one, thats the best I could do.
This one is driving me insane. Fought it years ago. Never did figure it out, gave up.

Anyways: simple side operation driven by an open curve.
Two rough passes, one finish pass. I am keeping the tool down between all passes.
But, I can't for the life of me get it to rapid back to the start of the next pass.
It returns at the same feed-rate it cuts. Tired if editing this damn program! (12 parts on the table)
I can't bi-direction rough (in the Brother). The tool has to climb (gets real grumpy conventional).

The only variable I can find that looks like it should affect this situation is "Min Rapid Distance %" in the milling tab.
But, it has zero effect on anything.

I am probably missing something stupid that has eluded me for 11 years! And, I am going to kick myself like an idiot when I figure it out.
I almost always am able to figure this shit out. But CRAP, I just can't win with this one!

Wheelie.


I know what you're after, but do not think it is possible without lifting the tool.
Yes, "Min Rapid Distance" would appear to be the setting for this, but it does not work. Never has AFAIK.
Actually, it is and has always been contradicting, as the "Z Rapid Plane " setting clearly says that below that surface no rapid movements will be allowed,
ergo, the Min Rapid Distance shall be ignored for X and Y movements.
Just tried to cheat it by putting in -1.0 for the Z Rapid plane and 0 for the Min Rapid Distance, and no, the tool will still feed back to the start point.


The only way I can make it rapid is if I uncheck " Minimize Tool Retract", but in that case it will rapid up-to the Z-rapid plane, rapid back, rapid down to Z-clearance, ramp-feed down the rest of the way in Z
and then starts the toolpath again.

I am still on V21, so do not know if there are any changes since ( have the new stuff but did not install it yet... )
But, I think the newver versions now have NT toolpaths for roughing as well and not just for finishing, so perhaps that might allow rapid ( or at least increased feed )
back to the start point without lifting ....

Like everything else in FC, there are about a dozen different settings that seem like they should affect this behaviour, and maybe one that might actually do something in any given situation.

What I have done when all else fails is to use "Optimise Feeds" to force it to increase the feedrate during link moves, ie. when tool load falls to zero.

You will have to play with this to get it right, but once you figure out how it works you can use it to effectively do what you're trying to do, except it will be a G1 with a high feedrate instead of a G0.

If you are running a high feedrate already (especially with HSM type paths) you will need to use the supersampling option with a big number, to make sure you don't subject your tool to any large instantaneous loads.

You can change the maximum percentage feedrate override to match your rapid feedrate if your control is capable. Most of mine will happily feed at rapid speeds if I tell them to.

wheelieking71 said:

Hard to come up with a good title for this one, thats the best I could do.
This one is driving me insane. Fought it years ago. Never did figure it out, gave up.

Anyways: simple side operation driven by an open curve.
Two rough passes, one finish pass. I am keeping the tool down between all passes.
But, I can't for the life of me get it to rapid back to the start of the next pass.
It returns at the same feed-rate it cuts. Tired if editing this damn program! (12 parts on the table)
I can't bi-direction rough (in the Brother). The tool has to climb (gets real grumpy conventional).

The only variable I can find that looks like it should affect this situation is "Min Rapid Distance %" in the milling tab.
But, it has zero effect on anything.

I am probably missing something stupid that has eluded me for 11 years! And, I am going to kick myself like an idiot when I figure it out.
I almost always am able to figure this shit out. But CRAP, I just can't win with this one!

Click to expand...

I am not familiar with Feature cam at all

HSMWorks also feeds back to the next cut when keeping tool down. They happen to have a high feed setting so you can "feed" back at near rapid. I was under the impression it was for safety purposes. I thought any XY rapids below the top of the model were done in feed (G1) to prevent the possible collision from dogleg moves.

Well, thanks for the sanity check at least guys. I guess I'm not as stupid as this was making me feel.
I will be testing a brand new post that I wrote tomorrow I guess I will edit all those rapids in again as well.
My butt-cheeks are sore from puckering already!

To the OP: have you put this operation in a sub routine so that you'd at most, have to edit it only once?

It is a tall order to expect general purpose software to be able to produce crash proof programs in EVERY situation that a routine might be used in (such as the dog leg rapid that may, or may not occur). And to trap for the times when such a move would be permissible, and when it wouldn't, would likely eat up more processing time and then users would be bitching how slow it is to post.

Sometimes, you just have to edit it to make it do what you want.

HuFlungDung said:

To the OP: have you put this operation in a sub routine so that you'd at most, have to edit it only once?

It is a tall order to expect general purpose software to be able to produce crash proof programs in EVERY situation that a routine might be used in (such as the dog leg rapid that may, or may not occur). And to trap for the times when such a move would be permissible, and when it wouldn't, would likely eat up more processing time and then users would be bitching how slow it is to post.

Sometimes, you just have to edit it to make it do what you want.

Click to expand...

No, I do do a whole lot of sub-routine stuff. Ironic really, because FeatureCAM's "multiple fixture documents" are the core reason.
The way they handle multiple fixtures is freakin' awesome. Until you have to hand edit code that cuts 12 parts in a row, LOL.

wheelieking71 said:

No, I do do a whole lot of sub-routine stuff. Ironic really, because FeatureCAM's "multiple fixture documents" are the core reason.
The way they handle multiple fixtures is freakin' awesome. Until you have to hand edit code that cuts 12 parts in a row, LOL.

Click to expand...

This drove me insane, I actually rewrote that section of code in my post to fix it. I've since gotten a new computer and a different job so I haven't messed with it in a while (or even know where that damn post went!). However I created a Post Variable exactly for this. Remember, there is nothing you can't do with FeatureCAM if you know what you're doing with the post....! I'm wondering though, could it possibly be fixed by adding leads (within the curve)?! I remember the lathe wouldn't post out canned cycles without adding lead in and lead out but I never tested it.