Help please...

[Brendan P]

ok, I have no choisce but to get my azz moving with X before I get left in the dust. I am having a simple problem with Backplot (which to this day I swear still sux).

I am doing a simple 2D contour. When I run the toolpath, it cuts completely around the part. However, when I run it in "backplot" it does not appear to cut on the inner circle. Or the 7.719 radius. It seems to just show it cutting a linear move in the X axis...WTF?

 

I have uploaded the file in the: MCX-MR2 or earlier folder called: 9260laser.mcx

 

If someone has a little time, can you verify this is happening to you as well and maybe why?

I dont know if it is a grafix card issue or what..

 

Thanks.

[gavetta]

Hey Brendan,

I opened it with X2 MR1 and yes it does exactly as you say. When I look at your lead in, lead out, you have it set entry>tangent>875%......maybe something there needs to change. I changed it to prependicular>0 length and also told it to enter/exit at mid point on closed contours and it went all the way around. Without the enter/exit at mid point on closed contours it still does what it did before. Weird. HTH

[Namliek_J@TheeCircle™]

Brendan,

 

I dont know why it is doing that, but to fix it....all you need to do is change your start point so that the first chain cut is the inner radius and it will work fine.

[mcpgmr]

What does it do in Verify? Does the code appear to be correct. No "X" here but I've see older versions do something like that. Back plot settings maybe?

[wfcPain]

It back plots correct using wear comp.

Using control ,it does not back plot correctly.

I dont think it's a graphic card issue.

I'm getting the same result as you.

[Namliek_J@TheeCircle™]

-------------------------------------------------

This is what I get when I post the code when the back plot looks incorrect:

 

N60T1M6

N70G0G90X5.0014Y2.8033S0M5

N80G43H0Z.1

N90G1Z0.F0.

N100G41X4.9324Y2.7911

N110X.4396Y2.

N120G2X24.6224I12.0914J2.1494

N130G1X20.1296Y2.7911

N140G3G40X4.9324I-7.5986J1.3583

N150G1Z.1

N160M5

-------------------------------------------------

 

This is what I get when I post the code and backplot looks good:

 

N60T1M6

N70G0G90X20.1296Y2.7911S0M5

N80G43H0Z.1

N90G1Z0.F0.

N100G3G41X4.9324I-7.5986J1.3583

N110G1X.4396Y2.

N120G2X24.6224I12.0914J2.1494

N130G1X20.1296Y2.7911

N140G40X20.1158Y2.7936

N150Z.1

N160M5

-------------------------------------------------

 

All I did was change the start point.

 

HTH.

[Randy Morton @ Clem Industrial]

I tried as well and it verifys nicely and backplots funny so I posted it with my haas post and it backplots in cimco properly... Very strange indeed. The suggestions listed above to remedy it are great but why should you need to adjust your cut (maybe to a less efficient way) so that MC will display it properly?

 

Something fishy to me. And to think,most of the time I prefer the backplot over the verify.

[Brendan P]

Thanks for verifying that I wasn't me having too many beers last nite!! LOL

This is why I'm having such a hard time transforming outta 9.1! I cant get the most simplistic things to work, how are the complex things getting done!

Ya think it is a BUG or something? I have ran my laser toolpaths like this on 9 with no problems... What is the bug report email? [email protected]? I always use "control" for my comp. He comps the laser beam at his machine.

 

BTW, How do you shut off the big thick RED feed move lines in backplot. I hate those.....

 

Thanks guys

[gavetta]

Brendan, I opened it up again after reading others suggestions and just set the comp to computer and left everything else the way you had it and it backplotted fine. Must be something to do with the comp. Weird still.

[Dan@home]

I changed the tool to a 1/16 emill instead a .008 lasser beam and it worked fine. Maybe its a tolerance issue.

[Roger Martin from CNC Software]

On the Lead In/Out page, uncheck Gouge check entry/exit motion (in upper-left corner of the dialog)

[Hardmill]

quote:

---

how are the complex things getting done!

---

Easily

Hey bonehead, why didnt you send your file to me. I woulda looked at it for you.

 

Gonna go down there and :SMACK: the hell outta ya.

 

 

PEACE

[Brendan P]

quote:

---

Hey bonehead, why didnt you send your file to me. I woulda looked at it for you.

---

Wasn't sure what place of employment to send it to. That changes like the wind with you!!

[Kannon]

quote:

---

Wasn't sure what place of employment to send it to.

---

I didnt think the taco stand had email

[Pat-TGM]

quote:

---

On the Lead In/Out page, uncheck Gouge check entry/exit motion (in upper-left corner of the dialog)

---

If you uncheck this button, The Tool will Gouge to the part at lead in/out line.

 

 

Brendan,

 

The problem is You use Cutter compensation in CONTROL.

 

Yours nc code look ok but you will get scrap part.

Zoom in corner where the tool starts and backplot with quick verify on you will see the tool gouge in the part . In your application (tool dia = .008") maybe cut in .0001". But if your tool Dia = 2.0" what happen ?

 

 

So to solve this problem in Lead in/out page,

 

If you use tangent, You must have some value BIGGER 1/2 Dia of Tool in red box in picture below or use perpendicular

 

 

HTH