[Chris Duncan]

Tormach 770
MC X4
SW 2010 part

Trying to finish machine a flat surface, trying several methods (face, surface finish parallel, flowline) but none will ignore two 13/32 holes. Want it to machine flat across without lifting and it's going up to the retract height as it goes over the holes.

Also will the generic mill in MC work with the 770 Mach3 controller?

Is there any way to "verify" a complete Toolpath Group? I can do them one at a time but not all in order.


Attachment 222372

[Bm150]

Either make a surface same as face without holes. Or fill holes with surface. Look through the menus and should fund it. I will add picture when I get chance if you still have no luck.
Then add these surfaces to your drive.
Can't help with mach controller sorry.
Should be able to verify what you want. As long as it has a tick in the operation manager then it will be verified.

Sent from my HTC One using Tapatalk

[Chris Duncan]

Tried to make surfaces to fill the holes in MC but don't think I had them in the drive selection because it still wouldn't ignore the holes. Eventually just made another part in SW without the holes so have to load the NC separate from the hole NC.

The generic MC mill will work with Mach3, I did a mock run of all the operations and drilled the holes but Mach rejects the higher tool numbers, like anything above 200. Had to go in and re number them. Since I'm manually changing tools guess it doesn't matter.

I can verify all the individual toolpaths, but only one at a time, and it always starts with an original piece of stock. My only other experience with CAM software was with SpruteCam and with that you could do all paths at once and it showed the progressive machining from each previous operation.

That brings up another problem. I wanted an odd shaped piece of stock so built an STL in SW and brought it in under the stock settings. It shows in the display but when running verify it reverts back to a generic rectangular piece of stock.

Maybe X7 has some improvements. Maybe the boss will go for an upgrade, maybe...

[Tony T]

To verify all cuts simply select them all then enter verify. Once in verify in order to use your stl you will have to change within. Before you click run click on the folder icon and it will bring up options page, click on stock to use as file then navigate to the file you want to use. x7 is suppose to be able to be verified with stock showing from previous ops? I haven't made the switch so I don't know for sure. The only way in x4 is to save your cut stock as a stl before quitting verify.

[Superman]

Trying to finish machine a flat surface, trying several methods (face, surface finish parallel, flowline) but none will ignore two 13/32 holes. Want it to machine flat across without lifting and it's going up to the retract height as it goes over the holes.

- Have you tried doing it with the basic 2D contour ( use a single wireframe entity,,, no surfaces or solid faces )
- There is a fill hole command under the Surfaces pull-down, what it does is create a patch over the hole, that patch is also selected to be machined to make the toolpath continuous.
- You can create a surface from the solid, then remove holes on that surface

Also will the generic mill in MC work with the 770 Mach3 controller?

generic mill ???,
- normally, a specific "CNC_Machine" ( say it can be named "generic"), is a collection of other files ( .CONTROL & a .PST ) ,so that by selecting this generic mill, the necessary files & settings are used to create an NC file that is correct for that cnc machine....
- I assume you mean the Generic Fanuc 3 axis post ? yes, but you need to ensure that all things ( NC code ) that are output, will drive your machine correctly.

Is there any way to "verify" a complete Toolpath Group? I can do them one at a time but not all in order.

- click on the machine name, should select all operations under that machine
- same happens if you select by clicking the "toolgroup"

you can select individual operations, it uses the normal window command keys
- L/click your 1st operation, then [shift+ L/click] the last operation will select it and all operations in between.
- L/click one operation, then [control + L/click] will add or subtract ops to the group selection ( this works also when selecting whole "toolgroups")



I do think there is another ( faster) way to do your part
- Face the whole part to the top face ( to Z0.).
- Contour front area to the stepped face, up to the start of the lower radius.
- Contour front step with bull nose cutter same radius as on the part.
- Contour the upper radius with a corner rounding tool.

Why try to surface any feature , if it can be done with 1 pass using an off the shelf, standard tool
- surfacing does make larger files, and can make cycle times extremely long.
- surfacing should only be done if no other cost effective solution exists ie you don't have tooling to create those shapes.

[Chris Duncan]

Found the hole fill. I had already made a non-hole part in SW but next time.

Sorry, used the wrong word, not generic. Machine Type. MILL DEFAULT.MMD

found the group verify

I'm new at this. Agree with you on surface after doing it this way. LONG run time. The radius is not a standard increment but it wouldn't hurt the design to make it so.