Can't keep tool down in pocket remachine

[Thad]

Can anyone tell me what I'm doing wrong here? I can't seem to get the "keep tool down" feature to work. I have put a file on cadcam's FTP called remachine.mc9 in the V9 folder. It's a simple 2D pocket that ruffs and then remachines the corners.

 

Thad

[Reece L Gibson]

Set your "Retract" and "Feed plane" to zero and click the "incr" button.This keeps the tool down(in this case) in betwwen passes.

It will not raise above Z0 when moving to to next section which is kinda risky, assuming the pocket has already been cleared out.

[Thad]

Millturn,

 

Am I correct in assuming that this is a workaround, not the way keep tool down in supposed to work? It seems to me that just by checking off keep tool down, that in itself, should do what I want.

 

As far as the tool retracting to Z0 (top of part) before moving to next corner, I agree it's risky, but would probably do it if *I* was running the programs. The way we're set up, I do the programming and the guy down on the floor runs them.

 

Just for grins, I created another pocket and machined it the same way. The tool retracts to a clearance in between pockets.

 

Thad

[Thad]

Anyone else?

 

Thad

[cadcam]

Thad at this time I am with Millturn there is no other way at thsi time for remachine.

 

Send this thought to [email protected] about the Keep tool down button not doing anything.

[Thad]

If thats the way "keep tool down" is supposed to work, it's pretty weak. By making the changes that Millturn suggested, the tool will stay down whether "keep tool down" is selected or not. That's why I suggested that maybe it was a workaround.

 

I have contacted my VAR about this and it was forwarded to CNC Software in early July. Still no response.

 

Am I the only one in this forum that wants to use "keep tool down" in a pocket remachining cycle? C'mon, somebody help me out here.

 

Thad

[d0gFartz]

Good luck....im still waiting to be able to select a different tool when you enable create additional op.............i guess im the only guy in the world who roughs with one size mill and finishs with a different size end mill

[PE @ IHS]

Perhaps I am way off mark here...when machining a pocket, you naturally want to keep the tool down to eliminate unnecessary Z moves (up and down). When doing re-machining, keeping the tool down would enable you to rapid in X and Y to the next location within the pocket, thus risking breaking the tool by rubbing on the finished depth during rapid. Perhaps this feature is purposely not enabled during remachining, since this op generally involves the tool moving in rapid from one location to another within a pocket, which you wouldn't want to do in rapid mode unless you retracted in Z.

 

Peter Eigler

[Thad]

quote:

---

When doing re-machining, keeping the tool down would enable you to rapid in X and Y to the next location within the pocket, thus risking breaking the tool by rubbing on the finished depth during rapid. Perhaps this feature is purposely not enabled during remachining, since this op generally involves the tool moving in rapid from one location to another within a pocket, which you wouldn't want to do in rapid mode unless you retracted in Z.

---

Peter,

 

Before the tool moves from one location to the next (within the pocket), it goes to the "retract" level first...eliminating the crash potential.

 

Thad

 

[ 09-23-2002, 02:26 PM: Message edited by: thad ]

[Jerry Crofoot]

I have written a remachine toolpath that would not stay down and at other times I have seen it when it would stay down. I believe if the last toolpath written that had the option to "Stay down" and you exercise that option, then remachine will let you keep the toolpath down. If you did not exercise that option in the earlier toolpath, remachine will not stay down. If my last toolpath kept the tool up (example finishing a pocket), I have be able to write a dummy toolpath that held the toolpath down and then wrote the remachine toolpath in order to hold it down. After I get the remachine to work I delete the dummy toolpath. I agree that this is a software problem.

[McRae]

Thad,

 

Check out REMACHINE_MFGENG.MC9 on the FTP site and see if I understand your original intention. Please clarify the specifications first.

 

1) Disable depth cuts

2) enable finish in the tool path and disable rough

3) select keep tool down in the finish parameters dialogue box.

 

Peter - I tried the settings in the software and saw some cyan lines between corners. Feed, not rapid, and they are at depth. Look at it and see!

 

Will the all powerful SweaterMan software do what you ask? (this is for James' benefit, I really want to understand your question!)

 

Regards,

 

[ 09-23-2002, 03:14 PM: Message edited by: MfgEng ]

[McRae]

Also - What type of a tool changer do you have that would permit the tool to be changed without leaving the pocket of the part? Mine would have driven the tool thru the part and ruined my day!

 

It may function as you would like if the same tool was used for rough and finish, but then where is the remachine advantage? Still cloudy on the intent of the question.

 

Post Edit:

 

Further investigation, Set the stock boundaries and look at the verify, Do you want the remachine to recognize that there are radii at the intersection between the floor and walls as well?

 

[ 09-23-2002, 04:13 PM: Message edited by: MfgEng ]

[Thad]

Andrew,

 

I'll have to check out your MC9 file tomorrow. I left 5 minutes after I made my last post. To clarify the specifications, I NEED depth cuts and that's where I have keep tool down selected. I do not have finish parameters selected.

 

Will Gibbs do it? I don't recall. We only had the shop floor version that was resident in the Fadal control. It was always at least a version behind, even when you got a new machine. On top of that, since it came pre-installed, unless you got new "innards" for you machine, you still used the old version that came with the machine 5 years ago when you bought it. So, as luck would have it, remachining just came out "in our world" and our company closed shortly after. BTW, if anyone is going to rip on Bill Gibbs, they need to do their homework first. Suspenders and a tie has been his schtick for a while now.

 

Thad

 

[ 09-23-2002, 07:29 PM: Message edited by: thad ]

[Thad]

quote:

---

Also - What type of a tool changer do you have that would permit the tool to be changed without leaving the pocket of the part? Mine would have driven the tool thru the part and ruined my day!

---

I see some confusion. I ruff the pocket with a 1.5 cutter, then in another operation, I remachine the corners with a 5/8. When remachining, I want the tool to stay down between each .100 pass in the corner. The start point and end point of the remachine path in a single corner are less than an inch away (I'm guessing). I don't need the tool to rapid up, over an inch, and then back down. I want it to stay down and rapid back to the start point.

 

quote:

---

Further investigation, Set the stock boundaries and look at the verify, Do you want the remachine to recognize that there are radii at the intersection between the floor and walls as well?

---

No. That radius will get milled out when I finish the pocket walls (3rd op) anyway.

 

Thad

[Thad]

Interesting observation, Jerry! Does it do this for you consistantly? The best I've ever come up with was to get it to stay down on the last 3 corners of a square pocket, but it still retracts on the first. I've done multiple pockets and every time, it retracts on the first corner and then stays down on the other 3 corners. I couldn't get it to do it consistantly. Next time it comes up, I'll give your workaround a try. Thanks for the input.

 

Thad

[Thad]

Andrew,

 

Your file kept the tool down. Unfortunately, I need depth cuts when remachining.

 

Thad

[Thad]

Jerry,

 

I wasn't able to duplicate your situation. Do you have a file that you can upload to cadcam's FTP? V8 or V9.

 

Thad

[McRae]

Thad,

 

I have copied another file and appended depthcuts to the filename. Check out the parts, it will move across the floor of the part and then pop up to the first depthcut. I wouldn't want to run this program...

[Thad]

Andrew,

 

That's what I came up with when trying to duplicate Jerry's scenerio. Apparently, I'm SOL on this one. Thanks for your time.

 

Thad

[Jerry Crofoot]

Thad,

No I cannot do it consistently, but most of the time. If the remachined's stock is computed against the previous toolpath and previous toolpath held the toolpath down, it generally will also hold it down in the remachine toolpath if set to hold the tool down in the parameters. If the rougher does not stay down then I have never been able to hold the remachine down.

 

I have tricked the system by writing a dummy toolpath with the tool held down and then write the remachine toolpath against the dummy toolpath. Then delete the dummy toolpath and reattach the remachine contour to some other operation.

 

Once the remachine toolpath comes up, it is pretty hard to get it down without deleting the remachine operation and starting again fresh. Mastercam must be hanging onto to the last toolpath defaults and over writing the remachine toolpath hold down feature. I like remachine, it saves me a lot of time, but I wish I could hit it right the first and every time I use it.

[cadman268]

I used to do this in v7, go to the dialog to set gap settings and change to broken or direct for that toolpath, or change the percentage before it rapids. But don't forget to turn it back to default later.