BobCAD-CAM

Viewing post 1 to 10 (10 total posts)

just purchased version 25 . simulation for tool paths doesnt show cutter comp (10 posts)

← Group Forum Group Forum Directory

john said 10 months, 3 weeks ago ago:

how do i get version 25 to show the proper simulation in cutter comp.
my models always get shown with too much stock removal because the cutter doesnt comp over

#
Rob said 10 months, 3 weeks ago ago:

John

The software does the simulation correctly.

If you have set a “G41/G42″ in your feature then the “comp” is at the machine not in the software, you have set the software to generate the toolpath as the center of the cutter and that is where the simulation will show the cutter, it is accurate to what you set it to.

If you want the simulation to show you how the part will be cut then you should use the “Offset Left/Right” and then swap it back to your preferred “G41/G42″ when you want to generate the code for your machine.

Regards
Rob

#
john said 10 months, 3 weeks ago ago:

thank you . that works.

#
cheezewiz said 10 months, 2 weeks ago ago:

I didn’t want to be the one to bring this up (again). Is using machine compensation (G41/G42) just not used anymore? It does make it difficult to program the part one way for simulation, then make changes before you post code. It’s almost defeating the purpose of verification.

But if I’m one of only a handful of people programming this way I might have to just give in.

#
Rob said 10 months, 2 weeks ago ago:

You might just be right there “cheezewiz”, I think most folks don`t need to run the G41/G42 as they are probably able to run to “job tolerance” with the machine and cutter tolerances they have.

No often I need to do it either these days and to be fair most folks who are running to fine tolerances will most likely have automatic systems on their machines that will probe the part and alter the cutter offsets to get the required accuracy automatically and show it in full colour graphics simulation at the machine control

I`m still “wishing” for one of those

I do agree with you though, it is something that we could do with not having to do all the time

@BobCAD – - Wishlist Item please

Regards
Rob

#
jrmach said 10 months, 2 weeks ago ago:

I usually use BoBS compensation.In a lot of cases for me,I am on doing a couple of parts and I just inch my way towards the tolerance and repost new code each time I make an adjustment.Maybe not the right way, but it is just as quick almost.Got laptop right there at machine,it is already on and program opened.All I need to do is erase program,hit yes,receive program at the machine.Then usually change tool diameter(always use manual tools),compute toolpath,post edit cnc,send to machine.Sounds like more work than is.Do it all in 15 to 20 seconds.Like I said 1 or 2 parts usually what is ran.And alot of the the times when I do this I am also crossing out ops not to post the second run thru,so had to reload program anyways.As fast as the dnc downloads it really is almost as easy for me this way.This was my method for 23.Now 25 I may need to change things,for one thing haven’t they fix the problems now in the newer versions that were in 23 with using machine comp?

#
Bibi said 10 months, 2 weeks ago ago:

There’s a way to have the best of both worlds…hard code a G41 in your post on the XY Leadin (and G40 on leadout), but program with Bobcad.offsetting the path.

2 things you need to be sure of, 1…you always use “Offset Left” and 2….your tool offset is now treated as a wear offset. So you start at 0 and go +/- from there.

You guys remember way back to that awful 2007 release? That interface actually would allow a selectable combination of offsets similar to this…but too many “users” apparently couldn’t figure it out.

#
burr said 10 months, 2 weeks ago ago:

“”"”"”"”"”"”"”"”I didn’t want to be the one to bring this up (again). Is using machine compensation (G41/G42) just not used anymore? It does make it difficult to program the part one way for simulation, then make changes before you post code. It’s almost defeating the purpose of verification.

But if I’m one of only a handful of people programming this way I might have to just give in.”"”"”"”"”"”"”"”

The coded G41/42 is something being addressed with the Moduleworks provider at some level. Nothing BobCad can do until, trickles down.

#
cheezewiz said 10 months, 2 weeks ago ago:

@jrmach BobCAD V24 and V25 handles cutter comp really well, even allowing a side allowance when using G41/G42. Like Burr pointed out, it’s the verification side that’s never supported it. The Predator Backplot supports it, but man the Simulation is so much better.

Predator VCNC didn’t support it either. That’s why I ask if this is the direction everything is heading.

#
cheezewiz said 10 months, 2 weeks ago ago:

@Bibi I missed your post. Yes, that’s how I see people doing it these days. To my knowledge it works just as well. But @general hit right at my problem. The tool probe works with diameter, and it will need to know the starting diameter to check for wear. I’m doing a bit of research to see if the Renishaw macros can work with that style of cutter compensation.

I also know some folks that can do as jrmach does and just repost the code as the cutter wears. I realize at some point cutter compensation could even become obsolete!

#