[DMaz]

Hi all,

I've been using bobcad V25 Pro for a couple years on a mill that I retrofitted with a PC based control running Mach 3.

One thing I've not been able to figure out is, in the bobcad generated simulation of a program it "thinks" it's moving at a rapid feedrate (red lines) when the Z axis is above the part but the post will frequently and randomly have these repositioning moves running at G01.

I've tried varying the Rapid and Feedrate planes to no avail.

I'm using this post:

Mach3-Mill-NoATC.MillPst

but have tried the other MACH3 post that came with the program too.

This is a typical Piece of code:


N31 X-3.0709 Y-2.085
N32 G03 X-3.0435 Y-2.2479 I.0676 J-.0724
N33 G01 X-2.8839 Y-2.3188
N34 Z.1
N35 X-2.4593 Y.51
N36 G00 Z-.215
N37 G03 X-2.4593 Y.2107 I.6471 J-.1496 F15.
N38 G02 X-2.429 Y-.0443 I-1.1323 J-.2639
N39 G01 Y-.0495
N40 Y-.9307
N41 G02 X-2.5977 Y-1.178 I-.2657 J0.
N42 G01 Z.1
N43 X-2.7704 Y.51
N44 G00 Z-.215
N45 G03 X-2.7704 Y.2108 I.4697 J-.1496 F15.
N46 G02 X-2.729 Y-.0461 I-.8104 J-.2623
N47 G01 Y-.0495
N48 Y-.8479
N49 X-2.7178 Y-1.1462
N50 Z.1
N51 X-3.095 Y.51
N52 G00 Z-.215
N53 G03 X-3.095 Y.2108 I.2922 J-.1496 F15.
N54 G02 X-3.029 Y-.0478 I-.4865 J-.2619
N55 G01 Y-.0495

Lines 34, 42 and 50 all move to Z.1 but the next "repositioning" move is at G1 when it should be G0. Even more confusing, the G0 Z- moves following. It's like it figured out it should be in rapid 2 lines too late, lol.

I suffer through fixing these manually when I'm making many parts with the same program but when it's only a few then it can be a waste of time to try and fix the program manually as opposed to just letting the machine run.

This is also a somewhat random problem with the G0 moves occurring as they should maybe 10% of the time in a program.

Hopefully this is a post problem.

Any help is appreciated!

[magicniner]

I'm running V25 and have given up on finding a good off the shelf BCC Post for Mach3, or even finding good documentation for writing/modifying BCC Posts, I am gradually trying to work out where changes need to be made but the lack of good documentation isn't making it a particularly speedy process.
At the moment I'm working on why for Contour Ramping of Profiles the plunge feed rate is used for the linear feed rate except for the last pass, at the moment I just put the same value in plunge feed per tooth as feed per tooth.

[DMaz]

Thanks for the input. So are you inclined to think this is a post issue vs a bobcad issue?

Maybe I'll just start plowing through all the fanuc posts as all the commands are the same for the most part, at least for my applications.

As far as the ramping feedrate I just ran into the same issue a couple weeks ago. All I can deduce is that because there is ANY Z Axis movement it defaults to the plunge feedrate. The last pass has no Z movement so it sets the feed for this last pass to the normal G01 rate, it seems. I used the same fix, set plunge rate to G01 rate and go...

Funny, I've had to come up with so many of these little techniques or "work arounds" or whatever you want to call them to deal with the issues I've encountered that I forget them until the next time the issue rears it's head.

Maybe someone should start a Sticky thread called "Bob-Cad Work Arounds" so that it's easy to search for a solution to these commonplace problems.

Couple more...

Reverse or perhaps more appropriately, "Skipped" roughing cuts. Meaning, when using Advanced Rough it will sometimes, for no apparent reason, skip a roughing cut causing the subsequent pass to take a double depth cut (or more depending on how many roughing passes it "skips"), and then, at the end roughing cycle, it goes back and makes these missed cuts, cutting nothing of course... No fix for this one yet.

For my purposes the Advanced Rough is by far the most powerful toolpath Feature. There are lots of little things I'd like to see added like the ability to specify different Z vs. XY axis stock remaining for the finish pass, or even the ability to use tool offsets so that if the part size is slightly off I can adjust the tool size instead of re-posting the entire program with a new tool diameter, Ugh! Oh yeah, and then fixing all the clearance plane feedrate moves again, lol!

One thing that I've mentioned repeatedly to the Bob-Cad sales people who call pitching the Newer versions, is why the program can't "See" the material that's been removed for the next operation.

As a result, I VERY commonly save the machined stock from the CutSim tab in the simulator and start a new file beginning with this saved STL file as the new stock. At this point I can use the Advanced Rough again with a "0" value for stock remaining and do the finish cuts. Overall this technique works well for preventing Bob-Cad from crashing the tool because it doesn't "See" the stock or the part (which it does well in Advanced Rough, assuming you select the whole part) but the downside is that you have to stitch together several or sometimes many programs depending on how complicated the part and how many times you had to save the next STL file.

The other downside, which brings us back to the original post, is that for all these programs, many (or in reality most) of the Clearance Plane repositioning moves will be at Feedrate not Rapid, not to mention the Z+ moves to the Clearance Plane, which post out at Plunge Feedrates, which are almost always lower then the G01 rate. For a single part it's almost never worth the time to fix these problems especially because you're changing G01 moves to G0 moves and a single mistake over what may be hundreds of line fixes, can crash the machine.

The upside is that sometimes we'll just stand there and watch the crazy tool paths and feedrate clearance moves and have a good laugh, which is never a bad thing...

[The Engine Guy]

Thanks for the input. So are you inclined to think this is a post issue vs a bobcad issue?

Maybe I'll just start plowing through all the fanuc posts as all the commands are the same for the most part, at least for my applications.

Use the standard BC_3X post, it is a "generic" Fanuc PP and covers most things with only a little "tweaking" required

As far as the ramping feedrate I just ran into the same issue a couple weeks ago. All I can deduce is that because there is ANY Z Axis movement it defaults to the plunge feedrate. The last pass has no Z movement so it sets the feed for this last pass to the normal G01 rate, it seems. I used the same fix, set plunge rate to G01 rate and go...

Isn`t that what it is supposed to do ? Ramping is just another way of plunging so that`s what I would expect, why would you need a "fix" for it ? ?

Funny, I've had to come up with so many of these little techniques or "work arounds" or whatever you want to call them to deal with the issues I've encountered that I forget them until the next time the issue rears it's head.

Maybe someone should start a Sticky thread called "Bob-Cad Work Arounds" so that it's easy to search for a solution to these commonplace problems.

Couple more...

Reverse or perhaps more appropriately, "Skipped" roughing cuts. Meaning, when using Advanced Rough it will sometimes, for no apparent reason, skip a roughing cut causing the subsequent pass to take a double depth cut (or more depending on how many roughing passes it "skips"), and then, at the end roughing cycle, it goes back and makes these missed cuts, cutting nothing of course... No fix for this one yet.

Never seen this happen, maybe you can upload a file that does it ? ? Only thing I can think of that would cause that might be badly selected geometry ? ?

For my purposes the Advanced Rough is by far the most powerful toolpath Feature. There are lots of little things I'd like to see added like the ability to specify different Z vs. XY axis stock remaining for the finish pass, or even the ability to use tool offsets so that if the part size is slightly off I can adjust the tool size instead of re-posting the entire program with a new tool diameter, Ugh! Oh yeah, and then fixing all the clearance plane feedrate moves again, lol!

You can easily use tool offsets ( eg G41 D1 ) and then if you have the facility to alter the tool diameter at your machine control, no need to re-generate toolpaths

One thing that I've mentioned repeatedly to the Bob-Cad sales people who call pitching the Newer versions, is why the program can't "See" the material that's been removed for the next operation.

Why not try doing a second/third Advanced Roughing feature and use the "Rest Roughing" option, it should then follow on from what the previous tool cut from the stock Works here, it`s what it is supposed to do

As a result, I VERY commonly save the machined stock from the CutSim tab in the simulator and start a new file beginning with this saved STL file as the new stock. At this point I can use the Advanced Rough again with a "0" value for stock remaining and do the finish cuts. Overall this technique works well for preventing Bob-Cad from crashing the tool because it doesn't "See" the stock or the part (which it does well in Advanced Rough, assuming you select the whole part) but the downside is that you have to stitch together several or sometimes many programs depending on how complicated the part and how many times you had to save the next STL file.

Using the STL from the sim make for big files and slow toolpathing/saving times, handy to have but I only use it if I absolutely have to

The other downside, which brings us back to the original post, is that for all these programs, many (or in reality most) of the Clearance Plane repositioning moves will be at Feedrate not Rapid, not to mention the Z+ moves to the Clearance Plane, which post out at Plunge Feedrates, which are almost always lower then the G01 rate. For a single part it's almost never worth the time to fix these problems especially because you're changing G01 moves to G0 moves and a single mistake over what may be hundreds of line fixes, can crash the machine.

The upside is that sometimes we'll just stand there and watch the crazy tool paths and feedrate clearance moves and have a good laugh, which is never a bad thing...

[magicniner]

Isn`t that what it is supposed to do ?

If the tool can only plunge at 1/20th the linear feed rate but the ramp generated results in 1/30th the feed rate it still sets the linear speed to 1/20th the linear feed rate giving a plunge rate of 1/60th what the tool is rated for.
Based on that I'm guessing - NO ;-)

Ramping is just another way of plunging so that`s what I would expect, why would you need a "fix" for it ? ?

BCC invites you to define the maximum Linear and Plunge rates based on tooling and then in profile ramping the feature parameters set descent into the material as either an angle or a depth per pass, why would it be acceptable for the maximum plunge rate for the tooling to limit the linear speed of the tool path?
As with so much else it's clearly NYOC ( Not Yet Optimally Configured ) and requires a workaround ;-)
I haven't tried V27 yet to see if they've fixed it there, have they?

[DMaz]

Just tried the BC_3X post. Same result. G1 Z+ moves followed by G1 repositioning, then G0 Z-, just like my sample code.

The Rest Roughing works OK for a one dimensional part, i.e. only one roughing tool and then to a complete finish, but not if the part has features that have been made in more then one operation. It's a nice feature but not a substitute for "seeing" the remaining stock and producing toolpaths based on what's actually there...

Will a single G41 DX statement at the beginning of a X000 line program (within the same tool of course) work? I though this might be a solution initially but there are so many approaches and position/direction changes that it seems the tool would need to be ramped on and off repeatedly throughout the program, I'm not sure... I have much more lathe experience then mill. It would be great if that was a fix for part size adjustments.

I've never had a problem with BobCad crashing, running slow or tacking a long time to post using STL files al all. Other then stitching programs together and fixing the clearance plane feedrate issue the STL is not that big a deal.

I'll try to find a program that had the reversed roughing issue. I don't think it shows up on the Bobcad simulation so I'll have to remember one and load it into the mill to make sure. I'm inclined to think it's not a geometry or selection problem as the part comes out correctly otherwise but who knows for sure.

By far my biggest frustration is the feedrate issue. It can turn a 20 minute program into a 35 minute program pretty easily. A new post or whatever that fixed this issue would be a game changer for productivity. I keep thinking that the right combination of clearance/rapid/feedrate plane values would work but I haven't figured it out yet...

Another related question. Using a mill to produce a hole (or other small feature) can you prevent the tool from exiting the feature and moving back to the clearance plane before doing the next layer down? This characteristic, in combination with the Z+ clearance move at feedrate has me always mentally gambling with the limits of tooling as far as plunge/slot depth of cut because it's so time consuming to move out of the feature at feedrate and then all the way back down. If the Z+ move was rapid, or could be prevented entirely before the next plunge it would be much less time consuming to take shallower and safer cuts. I've gambled badly resulting in broken mills playing this game.

Thanks for the help!

[The Engine Guy]

Test Ramped Profile cut in Aluminium with Carbide 8mm tool, code below shows the linear cuts are correctly moving way faster than the angled (2 degrees) plunge cut, can`t see anything wrong with it, software appears to have used the values set in the material cutting conditions correctly in this example anyway

(FIRST CUT - FIRST TOOL)
(FEATURE PROFILE)

(TOOL #1 - 8mm 4Fl 55 deg Merlin Carbide)
N20 T1 M06
N30 G00 G90 G54 X-38. Y28. S4000 M03
N40 G43 H1 Z30. M08
N50 Z2. (Tool rapids to 2mm above part)
N60 G01 Z0. F1168.4 (Tool plunges to Z0 at plunge rate)
N70 X-28. F2336.8 (Tool leads in parallel at linear rate)
N80 X28. Z-1.956 F1168.4 (Tool starts to angle plunge at plunge rate)
N90 Y-28. Z-3.911
N100 X-28. Z-5.867
N110 Y28. Z-7.822
N120 X28. Z-9.778
N130 Y21.637 Z-10. (Tool reaches full depth, finishes angle plunge at plunge rate)
N140 Y-28. F2336.8 (Tool now does linear cut at required depth at linear rate)
N150 X-28.
N160 Y28.
N170 X28.
N180 Y21.637
N190 X38. (Tool now leads out at linear rate)
N200 G00 Z30. (Tool rapids to full clearance at full rapids rate)
N210 M09
N220 M05
N230 G91 G28 Z0.
N240 G91 G28 Y0.
(END OF FILE)
(END OF PROGRAM)
N250 M30
%

[magicniner]

Rob,
I've run tests in V25 build 996 and results are as stated.
What Version, Post and Build generated yours?

[The Engine Guy]

Rob,
I've run tests in V25 build 996 and results are as stated.
What Version, Post and Build generated yours?

That might be your problem, I "rolled back" from 996 to 895 due to a number of issues with 996.

P.S. PP is the basic Bc_3x.MillPst

[The Engine Guy]

Just tried the BC_3X post. Same result. G1 Z+ moves followed by G1 repositioning, then G0 Z-, just like my sample code.

The Rest Roughing works OK for a one dimensional part, i.e. only one roughing tool and then to a complete finish, but not if the part has features that have been made in more then one operation. It's a nice feature but not a substitute for "seeing" the remaining stock and producing toolpaths based on what's actually there...

Will a single G41 DX statement at the beginning of a X000 line program (within the same tool of course) work? I though this might be a solution initially but there are so many approaches and position/direction changes that it seems the tool would need to be ramped on and off repeatedly throughout the program, I'm not sure... I have much more lathe experience then mill. It would be great if that was a fix for part size adjustments.

I've never had a problem with BobCad crashing, running slow or tacking a long time to post using STL files al all. Other then stitching programs together and fixing the clearance plane feedrate issue the STL is not that big a deal.

I'll try to find a program that had the reversed roughing issue. I don't think it shows up on the Bobcad simulation so I'll have to remember one and load it into the mill to make sure. I'm inclined to think it's not a geometry or selection problem as the part comes out correctly otherwise but who knows for sure.

By far my biggest frustration is the feedrate issue. It can turn a 20 minute program into a 35 minute program pretty easily. A new post or whatever that fixed this issue would be a game changer for productivity. I keep thinking that the right combination of clearance/rapid/feedrate plane values would work but I haven't figured it out yet...

Another related question. Using a mill to produce a hole (or other small feature) can you prevent the tool from exiting the feature and moving back to the clearance plane before doing the next layer down? This characteristic, in combination with the Z+ clearance move at feedrate has me always mentally gambling with the limits of tooling as far as plunge/slot depth of cut because it's so time consuming to move out of the feature at feedrate and then all the way back down. If the Z+ move was rapid, or could be prevented entirely before the next plunge it would be much less time consuming to take shallower and safer cuts. I've gambled badly resulting in broken mills playing this game.

Thanks for the help!

If all the milling operations are done as "Rest Roughing" operations then the remaining stock will be "built" to the final shape regardless yes? ?

I do fairly complex 3D Molds that way sometimes as they can be fairly large files when using the STL files all the time, often 200~300Mb

[BurrMan]

One thing I've not been able to figure out is, in the bobcad generated simulation of a program it "thinks" it's moving at a rapid feedrate (red lines) when the Z axis is above the part but the post will frequently and randomly have these repositioning moves running at G01.

I've tried varying the Rapid and Feedrate planes to no avail.

Any help is appreciated!

I dont have the file to look at, but be sure you are not mistaking rapids and feeds with link moves... (its just what it sounds like you are describing here.) In areas those red lines are link moves, and those arent controlled by a post setting like that.

If these are what you are describing, then this response covers alot of whats been said...

There has been alot of discussion regarding those moves and needing wanting more control over them. I know dev is looking at it... if more control comes. I would expect it in a newer version... most definitly wouldnt expect it for v25....

yup, falls under more control and power added, and not "wrong"...

There are other things being discussed in the thread i am not reffering to..... just the linking "feed" and more control of those.

[magicniner]

That might be your problem, I "rolled back" from 996 to 895 due to a number of issues with 996.

P.S. PP is the basic Bc_3x.MillPst

I was forced to update to 996 by BCC Support when I reported the issue of the standard simulation showing 5-axis moves on a 5-axis simulated machine when dealing with a 4-axis machine definition.
It transpired that the solution was to buy Pro Simulation as Standard was incapable of dealing correctly with 4 axes but I don't have 895 to roll back to :-(
SSDD
Nick

[The Engine Guy]

I was forced to update to 996 by BCC Support when I reported the issue of the standard simulation showing 5-axis moves on a 5-axis simulated machine when dealing with a 4-axis machine definition.
It transpired that the solution was to buy Pro Simulation as Standard was incapable of dealing correctly with 4 axes but I don't have 895 to roll back to :-(
SSDD
Nick

Ah, right, I have never trusted the Modulewerks (German) simulation so I never actually tried to build a simulated machine, just seemed a bit pointless when all I have ever really needed were clearances for part/fixtures/vises/clamps and they are easily done (More easily done in fact in Predator) which I normally use to backplot the G code anyway

Still, each to their own, I just believe that if my code runs correctly through the backplot I won`t have any mishaps, the Modulewerks often looks OK but the code can still be out so not a 100% simulation like the backplot

Maybe BC will let you download 895 if you ask them ? ?

[shred]

Likely a post thing. You could switch off the 'are G-codes modal' switch (or "output G-codes every time" or some such.. I forget exactly what it's called) to see if it outputs G01 or G00 for the problem-child lines. I had to bash on my post to get it to quit Z-feeding down from toolchanges because it thought it was still in G0 when it was actually in G1. There's a not-very-clear "reset" command that you can stick in the post that regenerates the G word if needed which I think is what I ended up doing.

[DMaz]

Engine Guy

"If all the milling operations are done as "Rest Roughing" operations then the remaining stock will be "built" to the final shape regardless yes? ?"

Uh, no.

The toolpaths generated by Rest Roughing are not the same as the toolpaths generated by a straight use of the Advanced Rough without using the Rest Rough feature.

Typical example is this Part and Stock. Roughed with a 1/2" mill with DOC of .1 and .010" stock remaining.

The result of using the Rest Rough feature to finish the part with a .375 mill, specifying the previous parameters and 0 stock remaining yields the Rest Roughed result. It misses the flatlands completely (blue areas)

Rest Roughing doesn't recognize flat features (at least sometimes if not always, and yes I had the Machine Flatlands button checked)

One of the best characteristics of the Advanced Rough feature is it's ability to see and cut to everything without crashing the tool into the part. If it didn't see/machine flatlands it would be MUCH less useful.

If the stock remaining is saved and a new program is written using this STL as the new Stock when you run the same tool (.375 mill 0 stock remaining) it finishes the part perfectly, flatlands included.

So no, not the same at all. Rest Roughing is a limited substitute for the powerful toolpath capabilities of the Advanced Rough feature.

Speaking to the whole Ramp feedrate, I have build 996 and get the same result as you but the result we're getting is the issue. A true "Plunge" ie straight down into the part will have a much lower safe feedrate then a horizontal profiling move. The issue lies in the lack of a 3rd feedrate choice, perhaps a Ramp Rate. If you are ramping at a shallow angle then a suitable feedrate will be much higher then a true Plunge rate and be equal or very close to a horizontal rate. Yes, you can just set the plunge rate for that specific operation to 90% (or whatever) of your horizontal rate but then you have to be careful that there aren't any other operations with that tool that could default a true plunge to the inflated rate. No, not a real big deal or anything but something to note and address, otherwise you'll wonder why your getting such a slow feedrate on your profile ramping operations, which is how I discovered this in the first place,


Burrman

I'm not sure what distinguishes a Link move from a Clearance Plane move (my name) but I'm sure that they should be at a Rapid Rate. I know this because when you view the simulation in Bobcad it tells you the total lengths of the Cutting and Rapid toolpaths and these numbers don't agree with what's posted. That's part of the reason I'm hopeful I can fix this in a post. Bobcad WANTS these moves to be rapid they just don't post that way.

Shred

I've never tried to edit a post. Where do I find these controls or parameter switches to which you're referring? It sounds like your tool-change feedrate issue is very similar.

Thanks!

[jrmach]

Just a quick comment,,,tool paths that end with the "word" ROUGH,,,are just that,a roughing tool path.

[DMaz]

"Just a quick comment,,,tool paths that end with the "word" ROUGH,,,are just that,a roughing tool path."

Hilarious!!! Like I said, nothing like a good laugh!

Thanks for the comic relief!

[jrmach]

Was not being funny.
You have brought up quite a few questions in this thread.I am only commenting on the fact I see no mention of using finishing strategies.
You seem to have an idea of how you want the software to work,,but you need to use the software the way it is intended to work for best results.
Using Advance Rough as the means to do "all" is not right.
It is a Roughing tool path.
Screw around enough with it and it may work eventually for rough and finish,,,,or go to the proper finish tool path and do it right.
BTW V 27 is bad a$$

[aldepoalo]

I want to jump in here on a few topics.

#1 Upgrade to the current version... well it's true the current software version has lots of new options in all aspects of the software. If you are running V25 you are 2 version back and lots of things have be updated and changed for the better. So when it works for you to get current I recommend doing it.

#2 As far as feed moves and rapid moves for repositioning. there is an option on the links tab to handle this. You can change it from feed to rapid move. That should just be that easy.

#3 Operation stock! This is what you are looking for to keep track of material as you go. Yes you can use rest roughing which is mainly an offset that is being applied to your model. With the current version you can select operation stock for most of the pro toolpaths. The operation stock is a user loaded solid or STL file. So you can save out your cut model and load it in as your operation stock. Op stock is uses as a 3D boundary for your toolpath and can be combined with boundary options and angle ranges to better target material for rest roughing, semi finishing and finishing operations. I would recommend downloading a demo of the current version and giving it a try.

#4 Feature request is how you get changes in the software. If you don't like how the feed moves are posting when using contour ramp, then report it. Recommend how you would like to see the software work. These requests go directly to development , Software Issue Report & Feature Requests | CAD/CAM | BobCAD-CAM | BobCAD-CAM

Most of us can think of a hand full of things we would like to see changed in the software. Have you voice heard by reporting something today.

[DMaz]

JRMach: My apologies, I though I sensed a bit of sarcasm in your comment as I've always wondered why there wasn't an "Advanced Finish" operation.

I do use finishing operations frequently when I believe they will generate the best toolpath for the given feature. The top edges of the gussets on the part pictured finished nicely with a ball mill and an Equidistant Offset operation. I just personally find that Bobcad is "smarter" using Advanced Rough and produces more intuitive results, not that it's the only tool in the toolbox.

Please don't get me wrong. I've never failed to be able to make a part, some of which I'd consider to be reasonably complex, using Bobcad and have only had to resort to manually coding on a few occasions (most memorably undercuts with a dovetail or keyseat cutter).

Al:

Thank you for your input. V26 was released literally within a week of my V25 purchase and I did download a demo but didn't see anything that made the upgrade look sensible for me anyway. I haven't looked into V27 but I will.

"#2 As far as feed moves and rapid moves for repositioning. there is an option on the links tab to handle this. You can change it from feed to rapid move. That should just be that easy. "

Is this only in V27? I don't recall this choice in V25 but I could certainly be missing something. If not do you have any suggestions (short of updating to V27) on how to address the feedrate moves i.e. the topic of my original post? Do you think it could be fixed with a post processor change or alteration or are you inclined to think the move rates are hardwired into Bobcad and the post is just doing it's job?

Thanks!