Printable View
Hi All,
I'm trying to cut a hex on the end on a small shaft. I'm roughing it using system comp, and finishing using machine comp. The finish pass is making a shape I can't even identify. What I see when I run the simulation is also what I am getting at machine. Anyone seen this before? I've done this in past without problems, this just started today. Nothing on my system is changed. Attached is the V25 file and my post. Any help would be great.
Tony
Take a look at comp in your finish pass set the same as first cut ----comp/left----machine/off and it seems to be OK
Tony
Can`t see anything wrong here, both cuts perform a hexagon shaped cut, I`ve run it through my Predator Backplotter as well and it worked fine, I made a bigger square stock and a smaller cutter so I could see exactly where the cutter ran, seems OK, both do a Hexagon shape and lead in/out OK, the first cut was correctly offset and the second cut ran on the centre line of the geometry as it should have done.
Here is the image from Predator.
Attachment 228086
Looks more like a wrong setting at the machine for your tool offsets to me :D
One thing I noticed, you didn`t have the Hexagon geometry set as a "Contour" to get the correct direction of cut (Climb Mill). I did set a "Contour" to get the Climb Milling correct :D :D :D
Here is the code generated using your PP :-
%
O00100 (HEX)
( PROGRAM NAME - HEX)
( POST - HAAS VF)
( DATE - WED. 03/12/2014)
( TIME - 11:05PM)
N01 G00 G17 G40 G49 G90 G20 G80 M31
( FIRST CUT - FIRST TOOL)
(JOB 1 PROFILE)
(ROUGH SMALL HEX)
( TOOL # 1 1/8 FLAT ENDMILL - STANDARD)
N06 T1 M06
N11 G90 G54 X0.2014 Y0.1299 S6000 M03
N16 G43 H1 Z0.1
N21 M08
N26 G04 P0.5
N31 G01 Z-0.02 F25.
N36 X0.1264 Y0. F15.
N41 X0.0632 Y-0.1095
N46 X-0.0632
N51 X-0.1264 Y0.
N56 X-0.0632 Y0.1095
N61 X0.0632
N66 X0.1264 Y0.
N71 X0.2014 Y-0.1299
N76 G00 Z0.1
N81 Y0.1299
N86 Z0.08
N91 G01 Z-0.04 F25.
N96 X0.1264 Y0. F15.
N101 X0.0632 Y-0.1095
N106 X-0.0632
N111 X-0.1264 Y0.
N116 X-0.0632 Y0.1095
N121 X0.0632
N126 X0.1264 Y0.
N131 X0.2014 Y-0.1299
N136 G00 Z0.1
N141 Y0.1299
N146 Z0.06
N151 G01 Z-0.06 F25.
N156 X0.1264 Y0. F15.
N161 X0.0632 Y-0.1095
N166 X-0.0632
N171 X-0.1264 Y0.
N176 X-0.0632 Y0.1095
N181 X0.0632
N186 X0.1264 Y0.
N191 X0.2014 Y-0.1299
N196 G00 Z0.1
N201 Y0.1299
N206 Z0.055
N211 G01 Z-0.065 F25.
N216 X0.1264 Y0. F15.
N221 X0.0632 Y-0.1095
N226 X-0.0632
N231 X-0.1264 Y0.
N236 X-0.0632 Y0.1095
N241 X0.0632
N246 X0.1264 Y0.
N251 X0.2014 Y-0.1299
N256 G00 Z0.1
N261 M01
( NEXT CUT - SAME TOOL)
(JOB 2 PROFILE)
(FINISH SMALL HEX - MACH COMP ON)
N266 S6000 M03
N271 M08
N276 G90 G54 X0.127 Y0.1299
N281 G01 Z-0.063 F25.
N286 G41 D1 X0.052 Y0. F15.
N291 X0.026 Y-0.045
N296 X-0.026
N301 X-0.052 Y0.
N306 X-0.026 Y0.045
N311 X0.026
N316 X0.052 Y0.
N321 G40 X0.127 Y-0.1299
N326 G00 Z0.1
N331 Y0.1299
N336 Z0.098
N341 G01 Z-0.065 F25.
N346 G41 D1 X0.052 Y0. F15.
N351 X0.026 Y-0.045
N356 X-0.026
N361 X-0.052 Y0.
N366 X-0.026 Y0.045
N371 X0.026
N376 X0.052 Y0.
N381 G40 X0.127 Y-0.1299
N386 G00 Z0.1
N391 M09
N396 M05
N401 M33
N406 G91 G28 Z0.
N411 G91 G28 Y0.
N416 T1 M06
N421 M30
%
Regards
Rob
:rainfro: :rainfro: :rainfro:
It must be something with the machine comp when changing comp on rough it gives the same bad cut
Contour,remove geometry,re-select geometry,BINGO
Good catch Rob
I always use contours when possible,jsyk
What are the benefits of using machine comp when cam programs are doing it for us? I know in old Bobcad programs on Cam side the word Contour would show up but I haven't noticed it in the newer programs.
Any thoughts on this would be good info.
Thanks
RAF
RAFQuote:
Originally Posted by RAF.
The "Contour" facility is available under the "Other" tab on the top menu. Was/is a handy facility for getting toolpaths particularly on profiles going in the desired direction, this can now also be done in the newer versions (V26) in the CAM tree at feature geometry level.
However one of the main advantages of using Machine Compensation for the finish cut is that it is then very easy to make small adjustments to tool sizes in order to get better sizing, mostly used on older ( Some not so old :D) machines that might have a little/lot of wear in them, allows adjustments to be easily made at the machine instead of altering things in the Cad-CAM software, re-posting the code and re-loading it to the machine, a very, very useful facility.
Even on some newer "budget" machines that have Linear Rails as opposed to the more sturdy and gib adjustable "box way" type need it, CNC machines are only spot on in theory, usually in practice they aren`t so some adjustment is often required :D :D :D
Regards
Rob
:rainfro: :rainfro: :rainfro:
Isn't machine comp to allow for cutter size variation in a production environment where the operator might not be familiar with CAD/CAM?Quote:
Originally Posted by RAF.
RAFQuote:
Originally Posted by magicniner
Yes, that is also a use for it, my post above only outlined one of the main advantagesthat`s all, there are of course others :D :D :D
Regards
Rob
:rainfro: :rainfro: :rainfro:
tool wear,machine wear(worn spindle,ball screws,etc.),holding tight tolerances.If you change tools,good chance it will cut slightly different.If you edit speeds and feeds,that can also change what the tool actually cuts.
Roughing tools,there is not a reason to use this,but no reason you cannot.If you are using re-grinds,then it should become obvious that using comp. would be a great way of altering the different size instead of doing it in the program.In Tony's example his roughing tool was his finishing tool.That really is not how it should be if he is using comp.2 different tools should be used.It might of been a one part and he did it out of convenience ???
If you are the programmer and the operator and you have the computer at your machine area,not really a big deal,you can just alter program,like lying about the tool size.BUT,that creates its own issues for setting up and running parts in the future.So it is best practice to draw the part nominal size,use nominal size for tools,and use comp. for dialing in to tolerance.
I have used system comp AND machine comp, and used D0.000 for that tools'l registry offset. That allows for some of the parts to be made undersize for plating and some on the number. A D-0.0030 offset for chrome and a D-0.0010 for anodize is about right. The program stays the same even G41. The roughing program would be G41 D0 (dont use registry) and the finish would be G41 Dnn (to use that tools registry info).
I never used to use system comp, I would only use machine comp, because I liked being able to read the program easier at the machine. after awhile, I started to feel that I ended up with more program issues that way. I hated programming centerline toolpaths, cause its a little harder to find the exact spot in the program I might want to look at, because you need to add or subtract half the tool, but if you allow the cam system to do its job, youll not need to troubleshoot as many things. sometimes its just plain worse to try fight the system comp. running D.0000 , then moving it -.0005 or +.0005 to tweak is easier in my opinion. somebody else might tell you something totally different, and its really up to you to find what you like better.
Hey guys,
Thanks for all the input. Daughter had to have emergency surgery so I been out a week. Shes doing good.
Rob, of course I have tool offsets set correctly :p Not sure why it works on your system and not mine. I tried it on 2 different PC's running V25. Same result. See the pics. What I see in simulation is what I get at machine. Same bad cut. Notice the green lines for final passes. It is like it is trying to compensate for the starting point of X and Y of each line. I did try and do the contour as you said. Same bad result. I found if I set cutter in BCC to .001" Diameter it seems to work. Why does BCC do that if I have it set to machine comp and NOT system comp? BCC should not care what my cutter is when machine comp is on, right?
There must be a setting somewhere in BCC to adjust this? As I said I made this part before and it worked fine. Now even the old program I used last time has the same bad results. I have not updated anything on BCC since before. Any other ideas?
Attachment 229452Attachment 229454
Tony,on your second cut use system comp and machine comp.It works and IMO,as Bobcad guy points out,has many advantages.
"Why does BCC do that if I have it set to machine comp and NOT system comp? BCC should not care what my cutter is when machine comp is on, right?"
It evidently does.
I usually never use machine comp,as I have computer right at machine and usually only making 1 or 2 parts.I will just edit program,BUT if I do use it I always use system comp too.Here is one big thing I always worry about if only using machine comp,what if I have a big number left in the registry from a previous job and I forget to set it right on the next job ?????If I am using system comp also the number will likely be small from job to job.
Yeah I have PC at machine also. Just going to do this with system comp. Was just hoping that someone would know whats wrong here. I made this same part 2 months ago and it WORKED fine. If it worked then, why not now? That's what's making me crazy.. hehe. Maybe someone from BobCAD could look into this. Al? Anyone? :D
I got different results today with your file than I got when you 1st uploaded it.Rob seems to have too.Consistency seems to be not.
OK,the old file worked in preditor and not simulation.That was done by using contours and circular lead.
Without the circular lead it is showing not good in preditor,But if you system comp with manual comp all the bad goes away in preditor and simulation.
Moral of story,if you use manual comp.,also use system comp.???????