Tool path stopping short

biglord4ever · Mar 18, 2019

I have a part that I'm running a trace tool path to engrave some lettering on a part. It simulates fine in Fusion, but on the part, it's stopping just short of finishing the path- maybe .005". I don't have an optical comparitor, but with ye olde' naked eye, the tip of the tool looks fine. I can't think of why it'd be stopping short and not finishing each character.

Machine is a Brother TC-S2C

DMF_TomB · Mar 18, 2019

biglord4ever said:
I have a part that I'm running a trace tool path to engrave some lettering on a part. It simulates fine in Fusion, but on the part, it's stopping just short of finishing the path- maybe .005". I don't have an optical comparitor, but with ye olde' naked eye, the tip of the tool looks fine. I can't think of why it'd be stopping short and not finishing each character.

Machine is a Brother TC-S2C

.
read the program and understand tool comp. most likely it is a tool comp issue. if tool comp not programed to turn it off it in general looks 2 moves lines ahead and if too many comments or non movement lines in between G41 and G40 it usually tapers down to zero the tool comp that is if its acting like a fanuc program

Booze Daily · Mar 18, 2019

How fast are you feeding? It could be a little tool pressure leaving the last little bit uncut.

Hazzert · Mar 18, 2019

DMF_TomB said:
.
read the program and understand tool comp. most likely it is a tool comp issue. if tool comp not programed to turn it off it in general looks 2 moves lines ahead and if too many comments or non movement lines in between G41 and G40 it usually tapers down to zero the tool comp that is if its acting like a fanuc program

Presumably he's doing a basic centerline toolpath. There is not cutter comp involved. My CAM system doesn't even offer that as an option for centerline geometry.

13engines · Mar 18, 2019

I got a feeling it's a setting in your CAM that's throwing this off, but if nothing can be found there, try this.

If you're running at a high feed rate, or even if not but just to be sure, you might want to run your machine in Exact Stop Check Mode, or use Single Block Exact Stop Check only on the code lines (blocks) that create the part of the letters that finish in open space without continuing on to other same letter features.

I've had somewhat similar problems like this on a mid 90's Fanuc OMC machine.

Dave

biglord4ever · Mar 18, 2019

15500 rpm 46.5 ipm

BROTHERFRANK · Mar 18, 2019

Add G61 Exact Stop Check, G64 to cancel back to Cutting Mode.

litlerob1 · Mar 18, 2019

This is the main problem with CAM jockeys (no offense, I am one) they have no trouble shooting skills. If a Manual Machinist ran into this problem, he would try to figure out why the Machine isn't doing what it's told. Needless to say, it wouldn't happen in the first place.

R

Bluejeep · Mar 18, 2019

if using a tapered tool sounds like the tool is running shallower than programed, or surface lower than expected.

Wsurfer · Mar 19, 2019

Trace tool path limited. I often drive the tool path using sketch geometry instead of the model edge. Like tangential extension in other tool paths.

biglord4ever · Mar 20, 2019

I was able to get one of the two paths to work by reducing the feed rate to 10.1 IPM.

(top bad, bottom correct)

The only things I can think of are either tool deflection or the machine isn't processing the code quickly enough at the higher feedrate. But since slowing the feedrate didn't fix the other trace toolpath, I'm not confident on either of those guesses.

13engines · Mar 20, 2019

I'm telling ya... jack your feed rate back up to where it was originally, manually stick a G61 in a line by itself right before the tool first plunges into the work, and put a G64 at the end of it all and it's going to fix your problem. If you're not running a Fanuc control, I'm sure other controls have the same Exact Stop Check Mode functionality, although it may be called something different. You'll just have to find out how to call it up.

I just noticed my Mori book calls this - Function For Accurately Positioning At The End Of Linear Movement. If that doesn't ring a bell for you I don't know what will.

G61 (Exact Stop Check Modal Command)
G64 (Return to Normal Cutting Mode)
G9 (Single Block Exact Stop Check) Works only on the line that it leads.

What Exact Stop check does, is it forces the the machine to wait until all the servo errors and lag have resolved before moving onto the next block. I can see in your part where you're starting and ending cutting, and you're right it's coming up short. Exact Stock Check will fix this.

I have a job where I create a 1/4" closed end slot which I come back to with a DA cutter to chamfer. The chamfer is big enough to do both sides at once, so I'm running in a straight line down the center of the slot at a high-ish feed rate. Without Exact Stop Check, you can see that the chamfer on the end radii of the slot is less then the one at the beginning. Same thing that's happening to you. I turn on Exact Stop and the chamfer is even on both ends.

I have another job in UHMW that is nothing more then three square 1/2" wide 1/4" deep slots spaced 1/2" from each other and each square path being one inch bigger then the previous one. These slots also have rounded inside corners so it's not a perfectly square tool path, but almost. There is a male and female version of this part that have to fit closely together. I run the job without Exact Stop Check and they will not fit together at all. Using the very same tool path and turning on Exact Stop Check they'll fit together perfectly. It's simply the nature of the beast. That being a servo driven machine tool.

This phenomenon of machine tools is spelled out in all the control manuals with vector traces and charts and you name it. Most of the time it doesn't matter, but I'm sure many around here have similar war stories as I do about needing to deal with this minor shortcoming. Thankfully the control manufacturers have supplied options to deal with it. There's also things like Look Ahead and my favorite mouth full... Quadrant Projection Compensation Function. But that's for another day.

Dave

DMF_TomB · Mar 20, 2019

majority of engraving i have done for over 4 decades i tend to go 1 to 10 ipm feed. yes if cutter and tool holder sticking out way too much it can easily deflect. and many cnc are not that accurate at higher feed rates.
.
sure engrave in less than 1 minute and spend a hour deburring and recutting and trying to figure out what went wrong. me i usually engrave in less than 10 minutes and am done. i find nothing worse than spelling errors. i spend more time double checking that
.
many a time i find to go faster you need to go slower. when they list maximum feeds and speeds they are just that maximum not the minimum settings.

biglord4ever · Mar 20, 2019

13engines said:
I'm telling ya... jack your feed rate back up to where it was originally, manually stick a G61 in a line by itself right before the tool first plunges into the work, and put a G64 at the end of it all and it's going to fix your problem. If you're not running a Fanuc control, I'm sure other controls have the same Exact Stop Check Mode functionality, although it may be called something different. You'll just have to find out how to call it up.

I just noticed my Mori book calls this - Function For Accurately Positioning At The End Of Linear Movement. If that doesn't ring a bell for you I don't know what will.

G61 (Exact Stop Check Modal Command)
G64 (Return to Normal Cutting Mode)
G9 (Single Block Exact Stop Check) Works only on the line that it leads.

What Exact Stop check does, is it forces the the machine to wait until all the servo errors and lag have resolved before moving onto the next block. I can see in your part where you're starting and ending cutting, and you're right it's coming up short. Exact Stock Check will fix this.

I have a job where I create a 1/4" closed end slot which I come back to with a DA cutter to chamfer. The chamfer is big enough to do both sides at once, so I'm running in a straight line down the center of the slot at a high-ish feed rate. Without Exact Stop Check, you can see that the chamfer on the end radii of the slot is less then the one at the beginning. Same thing that's happening to you. I turn on Exact Stop and the chamfer is even on both ends.

I have another job in UHMW that is nothing more then three square 1/2" wide 1/4" deep slots spaced 1/2" from each other and each square path being one inch bigger then the previous one. These slots also have rounded inside corners so it's not a perfectly square tool path, but almost. There is a male and female version of this part that have to fit closely together. I run the job without Exact Stop Check and they will not fit together at all. Using the very same tool path and turning on Exact Stop Check they'll fit together perfectly. It's simply the nature of the beast. That being a servo driven machine tool.

This phenomenon of machine tools is spelled out in all the control manuals with vector traces and charts and you name it. Most of the time it doesn't matter, but I'm sure many around here have similar war stories as I do about needing to deal with this minor shortcoming. Thankfully the control manufacturers have supplied options to deal with it. There's also things like Look Ahead and my favorite mouth full... Quadrant Projection Compensation Function. But that's for another day.

Dave

Thanks Dave. I plan on doing some experiementing with this.

I've been talking with Yamazen as well and they're talking to me about the Look Ahead option.

I'll post my results once I run my tests.

Hazzert · Mar 20, 2019

What sort of font are you using and what does your code look like? Is it tiny point to point moves along each letter?

Try a font like moorpark (should be a default windows font) and make sure it's outputting arcs and lines and see if that fixes some of the issues you're having.

13engines · Mar 20, 2019

Hazzert said:
What sort of font are you using and what does your code look like? Is it tiny point to point moves along each letter?

Try a font like moorpark (should be a default windows font) and make sure it's outputting arcs and lines and see if that fixes some of the issues you're having.

Yes-yes, Hazzert has a good point. Arcs-arcs-arcs. Besides all the Exact Stop Check stuff, a ton of little linear moves does not make for nice looking engraving. I've even seen that make a machine shake/vibrate if trying to run too fast. Looking closely at your lower part, it sort of looks like it's made with small linear moves. Could be the power of suggestion, but Hmmm.

I know in the rare moments that I've used CAM derived tool paths for something like this, (large logo engravings) there was a button in my CAM software to force it to use arcs when possible. Makes your programs a hell of a lot shorter too. If you're control is hurting for storage room, it also may keep you from having to drip feed.

Dave

mountie · Mar 20, 2019

Hazzert said:
Try a font like moorpark (should be a default windows font)

Moorpark is a font that comes standard with GibbsCAM. It can be downloaded from here: GibbsCAM Downloads * Customer Self-Service

Hazzert · Mar 20, 2019

mountie said:
Moorpark is a font that comes standard with GibbsCAM. It can be downloaded from here: GibbsCAM Downloads * Customer Self-Service

I'm a gibbscam user so that would explain my familiarity with it then.

biglord4ever · Mar 24, 2019

Ran my test this weekend.

Original code with high feed rate- rounded corners, poor detail
Look ahead M260- less rounded corners than original, still not good enough
G61- PERFECT!

Thanks for all the help.

Tool path stopping short

Aluminum

Diamond

Titanium

Stainless

Stainless

Aluminum

Stainless

Diamond

Hot Rolled

Cast Iron

Aluminum

Stainless

Diamond

Aluminum

Stainless

Stainless

Aluminum

Stainless

Aluminum

Similar threads