Need Help X5 Multi Pass Contour in X5

[riseandgrind]

Hello everyone. Great forum. Lots of good information. 

 

Need some help if possible. I just got my HAAS VF0 up and running. This is my first CNC mill and I have been reading and watching lots of videos on how to program parts. I currently have a part I have designed in X5 and need a little help with some contour tool paths.  I will try my best to explain what I need help with.

 

1. I have a piece of 6061 stock 1.25" Height (Z axis) I want to make a contoured profile to that part. I wish to make 4 passes at Z-.3 depth of cut for the first 3 passes with a final pass of .4

  * I also want to leave .010 on the wall of the part so I can come back for a finish pass. This first op I want to use a YG 3 flute roughing end mill

  * For the finish pass I would just make 1 depth pass at Z-1.3 since it's a .010 cut on the wall of the part.

So if I understand this correctly, I would want 2 operations or toolpaths created in order to do this. The first pass would be my 4 multi passes to achieve my final depth leaving .010 on the wall.

The second tollbooth/op would be a depth of Z-1.3 and I would leave 0. on the wall for the final size.

 

So my question is, Im not quite sure I understand the menu options

 1. I obviously know how to select my tool, select the spindle speed and feed rate, lead in and lead outs and putting coolant on. Should I use the Computer or Wear option for the tool?

 

I am just not quite understanding the options. under multi pass do I choose 4 and a minimum depth of cut at .3?

I saw an option that said "stock to leave on the wall" I chose .010 for the first rough pass, then on the second pass I chose 0. Just not sure Im doing it right. 

 

Any help would be appreciated

 

 

 

 

[riseandgrind]

So I think I might have figured this out. Please feel free to correct me if I am wrong.

 

For my first Rough Pass Countour I chose max Rough Cut .3

Number of Finish Cuts 1 and Finish Cut .4

I left .01 stock

 

Then under linking Parameters I selected my depth at Z-1.3

 

Under Backplot it made 4 passes and appeared to leave the .01

 

I created another contour pass, but this time I unchecked Multi Pass and made the stock left 0.

Then in Linking Parameters made it Z-1.3

 

This appears to have achieved my desired results.....Is that the correct way for a simple contour path?

[BCW]

It sounds like you have it right, although I would normally maintain a constant depth of cut instead of going deeper on the final pass.

What do you put in your D value for a 1/2 endmill? This will determine whether you want wear, control, or computer.

 

Computer = Cutter comp is hard coded in the program and cannot be controlled outside of mastercam, G41 is not posted.

Wear = D value starts at 0 and if you have tool wear you would offset your D value -.001 for example.

Control = D value starts at your tool radius as a positive number.

[riseandgrind]

Thanks for the reply. I have not currently cut anything on my machine yet. My understanding is a 1/2 endmill has .02 ground so it's actually .48 in diameter.

I understand what you are saying about equal depth of cuts, the first parts will need to plunge just past  1.25 so I can use a double bevel chamfer tool, all future machined parts will be screwed down to that jig. I need the extra clearance to allow the chamfer tool access to the bottom of the part.

 

I know these are totally basic questions, but keep in mind this is my first CNC machine and I am trying to figure this out all on my own

 

I really don't know weather to use Computer Wear or Control. These parts don't have to be highly accurate. Im just trying to understand it all.

[taperlength]

I think you want "Depth Cuts" as well as "Multipass" just for the finish pass.

Open the Depth Cuts page of the tree and click the check.  

For max rough step, enter .3

# of Finish Cuts enter  1

Finish Step   enter  0.1

 

Then go to the Multipass page.

Rough

   Number  enter  1

   Spacing  enter  0

 

Finish

   Number  enter 1

   Spacing  enter  .01

 

Machine finish passes at

    (click) Final Depth

 

 

Do a Backplot or Verify  to try it out. 

[BCW]

I don't know if this is standard elsewhere but here in Maryland at the few shops I've worked we prefer wear mode. IMO it leaves less room for error having all 0's in your tool offset page. What is easier to look at and/or spot a mistake for you?

 

Wear mode:

-0.0000

-0.0005

-0.0000

-0.0002

 

or

 

Control Mode:

0.2500

0.1245

0.5000

0.3748

[The Cathedral]

Control mode was good when we were writing programs by hand as we just had to put in part dimensions. However now that it's almost all written on a computer, wear is the way to go. We use wear exclusively here.

[riseandgrind]

Thanks for all the replies. Today I got my flood coolant all mixed up and into the coolant tank. I was able to Spot Drill, Peck Drill and Tap a 5/16 18. That program was short so I simply printed my G-Code and inputed it by hand. Hopefully tomorrow I will be able to make my first chips. I bought a little kit that included the RS232 Cable, USB Adapter, Tester and a Null Modem Adapter. Hopefully I can get the HAAS to accept my .NC files. 

 

I am running Windows 8 64 bit. I have read that 64 bit can be finicky when using a USB to Serial Adapter? Was hoping to just send the files VIA Masterdom X5, but I also watched someone online do it through Hyper Terminal. Ideally I would like to use my MacBook Pro. I can design all my parts inside on my desktop then transfer the files to my macbook, take it out to my shop and plug in the USB adapter and send the files to the HAAS. Any programs I can use for the Macbook Pro?

[Allan]

Brand new mill (first CNC) and running 4 and a half year old software?

You might want to talk to your Mastercam dealer about the current offerings.

 

Allan

[Gloves]

we currently use X5 here as well and from most of the posts you are doing it the same way I would have. As for the cutter comp, we use wear on our Haas and we use control on some other machines.

I can tell you from experience here that "Wear" is the way you are going to want to go. That gives the operator the control to tweak the offset as needed at the machine.

 

Control doesn't seem to give the same.

 

we here are also moving to X9 this week actually, we just had to wait for upgraded machines due to the requirements ram wise. currently I have 6 gigs of ram and x9 that I am testing runs very sluggish.