[Andy Graves]

Nested a job onto two sheets of material. Thought I wouldn’t have enough but fortunately, it just barely worked out.

Check out the picture and you can see how little material was left. I am sure that if we would not had the CNC, we would have needed more material.

[Seth Emery]

Nice job, Andy! It’s great when the material layout works out this way and you don’t have to put any remnants into inventory.

[Steve , NY]

Andy, what program are you using ?

[Andy Graves]

Remnants are no good unless they get used, then it’s awesome.

We use AlphaCAM that does the CAD and CAM (toolpath).

[Steve , NY]

I’m using Alphacam V7.5 .       I got a question for all:  at the end of the program I would like the cnc to go all the way to the back so we can unload, right now we run the cnc back manually, can anyone point me in the right direction? I might have to manually type it into the end of the G-code.  We are using an Andersen selexx chief cnc.

[Andy Graves]

Posted By Steve , NY on 10 Aug 2013 02:09 PM

I’m using Alphacam V7.5 .       I got a question for all:  at the end of the program I would like the cnc to go all the way to the back so we can unload, right now we run the cnc back manually, can anyone point me in the right direction? I might have to manually type it into the end of the G-code.  We are using an Andersen selexx chief cnc.

Funny you mention this. I have the same issue where it parks at 0,0 when complete.  I want it to park at 144,60 so it gets out of the way.

I am sure there is a setting in preferences because it has to be written into the code of each job. Just not sure. 

Could it be that it needs to be set in the CNC machine software and not the CAD/CAM software?

If you figure this out, I would love to know.

Thanks,

Andy

[Steve , NY]

Andy,  could you make a very simple drawing and assign a toolpath to it and then E-mail the g-code to me.  I would like to compare it side to side with one of mine and see if I can figure out if the reason your cnc goes to 0,0 and mine doesn’t is in the machine and not in the cam software.   Thanks.

[Andy Graves]

Hey Steve,

I sent an email with two files.

Let me know if you do not receive it.

Thanks,

Andy

[Steve , NY]

Hi Andy,  I think I got it. 

Find the file “Licomdat” on your computer, select the “RPOSTS.ALP” folder, this is where your post processor is stored, double click on the one you are using, scroll down to where it says “Main Program TRAILING lines“. About the second or third line from the bottom it currently says:  G00 X0. Y0.    change the x and y values to where you want the cnc to go. (e.g.  X60. Y144.)  now save the changes.

  Now open your Alphacam software, click on the’ File’ tab, scroll down and click on the ‘Select Post’ tab, this will take you to the “RPOSTS.ALP” folder, select the post that you have just revised (check revised date). Done.   

Now go to Alphacam and print out a G-code and compare it to the G-code you sent me yesterday, the second to last line should now display your updated values instead of  G00 X0. Y0. 

Make sure you enter a period behind your x and y values.

Now I need some information from you.    Where is your ( G00 X0 Y0) line entered at under ” Main Program TRAILING lines” ?    Is it before the ‘ $MODAL ON’ line ?    Or between the ‘$ENDIF ‘ and the  ‘ ‘ sign ?  Or after the  ‘  ‘ sign ?

Hopefully this makes sense to you, if not let me know. Thanks for your help !!

[Steve , NY]

I ran a couple programs this morning with my revised post, works perfect, cnc goes all the way back as soon as it’s done with the program.

[Andy Graves]

Hey Steve,

Works great on my CNC as well. In fact, this will be great when I cut repetitive parts on a jig. Just copy the post and create a new park position. That way it will park out of the way but close enough to save time on the travel.

I sent you a file via email for the information you requested in a previous post.

Thanks for the help on this. I’ve been racking my brain for years trying to figure this out.

[Steve , NY]

If you are cutting parts on a jig, rather than change the post every time, it may be quicker to just edit the x and y values in the second to last line of the G-code before sending it to the cnc.

[Guy Robertson]

Andy,

There should be an area in your post processor to add “footer” info that will be appended to every program you make.  

I will have to look at our post to our Andi when I get into the office to see what ours is.  Our Northwood does this and so does our Andi, so I’m sure yours can also.

[Jon Olson]

Andy that is perfect. That’s how Serling does it. That’s ow you beat the system .more top less stock.

Great job

[Len Smith]

Good stuff here.

[Author]

Posts