Author Topic: CamBam plus 0.9.8  (Read 102329 times)

Offline EAC

  • Storm Trooper
  • ***
  • Posts: 179
    • View Profile
    • Eureka Airctraft
Re: CamBam plus 0.9.8
« Reply #135 on: February 13, 2011, 21:34:05 pm »
Ben,

It done that way so 9.7 and 9.8 can be loaded at the same time.  Some people go back to 9.7 from time to time, and some people are still working in 9.7 til they fully learn 9.8

Don @ EAC

Offline mhackney

  • Ewok
  • *
  • Posts: 24
    • View Profile
    • The Eclectic Angler
Tab oddity
« Reply #136 on: February 16, 2011, 14:43:18 pm »
Hi, I am using the latest 0.9.8 release to make flat disks (.032") in brass that I cut using Mach3 on a Sieg X2 minimill. I use 2 tabs on these disks (about 3" in diameter) to keep them in place. The odd thing is that when I cut the parts, the first tab doesn't get made or it is much smaller than I programmed it to be. the 2nd tab turns out perfect. I have tried several different test parts, used tangential lead in (the first tab gets cut right at the start of the program) and even move the start location away from the first tab. In all cases that "first" tab is not the proper size. I'll post the code when I get home tonight but wanted to check if this is a known problem that others have experienced.

cheers,
Michael
Learn how to make fly fishing reels! www.Reelsmithing.com

Offline pixelmaker

  • CNC Jedi
  • *****
  • Posts: 1788
    • View Profile
    • pixelmaker
Re: CamBam plus 0.9.8
« Reply #137 on: February 16, 2011, 15:54:22 pm »
hello mhackney

no, I have no problems with the tabs.
Perhaps you can upload a .cb file that we can see it?


Offline c.sitas

  • CNC Jedi
  • *****
  • Posts: 573
    • View Profile
Re: CamBam plus 0.9.8
« Reply #138 on: February 16, 2011, 15:59:21 pm »
Hello  mhachney;   I had this once and it turned out to be my set up .  Everything was not "dead nuts on". I reset my Z axis to as near perfect as I could. The problem went away. This is just a thought. c.sitas

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Re: CamBam plus 0.9.8
« Reply #139 on: February 16, 2011, 16:48:38 pm »
Hello,

I had this problem with slim parts, but it is not related to cambam, my part is pulled upward by the spiral of the mill and it cuts the tab in passing.  ::)

++
David

Offline blowlamp

  • CNC Jedi
  • *****
  • Posts: 1183
    • View Profile
Re: CamBam plus 0.9.8
« Reply #140 on: March 16, 2011, 09:04:39 am »
I'm having a few problems machining a mould with the attached file.
The picture shows that CamBam is causing a small overcut at the pointy end if I use any postprocessor other than Default.
The opposite end also cuts in an odd way, but might be to do with the step on the model of the part.



Martin.

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6209
    • View Profile
    • Cambam V1.0 French Doc
Re: CamBam plus 0.9.8
« Reply #141 on: March 16, 2011, 13:45:45 pm »
Hello Martin,

I try your file and get same problem with CV, and CNc simulator say an error on the file !!

I look the toolpath with step by step in CV with trace "on", and toolpath seems to be right  ???  ... you have this problem on the real part ? or just on simulation ?  maybe a CV bug ?

Edit: it's not possible to obtain this square angle with the mill !!

++
David

Offline 10bulls

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 2164
  • Coding Jedi
    • View Profile
    • www.cambam.info
Re: CamBam plus 0.9.8
« Reply #142 on: March 16, 2011, 21:33:23 pm »
I found the lines where CV was having that glitch, created a small gcode excerpt and loaded that into Mach3.
This loaded OK and the toolpath looked good.

There was a rather large diameter arc there, so hopefully this is just a precision glitch in CV.

I just reduced the maximum arc radius setting in my Mach3-CV post processor from 100000 to 10000 and reran the file.  This worked OK in CV with no snaggles.

I think the opposite end is due to the stepover setting.  You could try reducing the stepover or adding a roughing clearance to prevent it overcutting that bit.

Good luck!


Offline blowlamp

  • CNC Jedi
  • *****
  • Posts: 1183
    • View Profile
Re: CamBam plus 0.9.8
« Reply #143 on: March 17, 2011, 09:12:59 am »
Thanks for looking at that for me, Andy.

Changing the MaximumArcRadius fixed the overcut problem at the rounded end, but my fiddling with the StepOver setting hasn't sorted out the problem at the other end.

Due to how I've got to make this part, it won't matter because I've got to cut this longer than really needed and then trim it back anyway.

Here's another file that's been giving me some jip, because it's struggling with the LeadIn moves in two ways.

The first problem is shown in the picture as an overcut on the corner of the part (which I think is related to ToolDiameter and the MaxCrossoverDistance).

The second problem shows as an error message when I set AdjustCutWidth to True under the SideProfile option.

Thanks again.

Martin.

« Last Edit: March 17, 2011, 10:55:20 am by blowlamp »

Offline 10bulls

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 2164
  • Coding Jedi
    • View Profile
    • www.cambam.info
Re: CamBam plus 0.9.8
« Reply #144 on: March 17, 2011, 18:25:34 pm »
It is indeed the MaxCrossoverDistance to blame.

CamBam is just following orders! ( ::) ) in that the lead in start point is ~4mm away from each layer's toolpath end point.  The tool is quite large relative to the size of the part so a 0.7 MaxCrossoverDistance x 10mm tool diameter is 7mm.

That means the post processor is 'allowed' to do a feed move when the start of the next toolpath is within that distance from the end of the previous toolpath.

Reducing the MaxCrossoverDistance to 0.4 (4mm with a 10mm cutter) makes the problem go away as the distance back to the lead in start is larger than the max crossover distance so a plunge via the clearance plane is forced.

I think the naughtiest thing is that CamBam does not display the crossover feed moves (these are currently insert by the post processor code, after the toolpaths have been generated).  Displaying these moves is on the TODO list.  As well as giving a better representation of the actual toolpath this will also help improve the cutting time estimates.