how does control work

[cob]

what and when do you use control in mastercam.
I use the wear most of the time
I am starting to use computer
but I would like to know how CONTROL works.

[Joesph Jackman]

what control does in Mastercam is allow you to input the entire radius of the cutter in the CNC control diameter offset page. using control makes it a lot easier when you want to manually edit your program at the cnc control because your positions in the g code program will match the numbers on the print. the disadvantage if if forget to enter the radius of the cutter in the cnc control diameter offset page you will more often than not scrap the part, were as with wear you have a much better chance of not scraping the part. make a simple rectangle. contour it using control. post the program and compare the numbers to your print. do the same thing and use wear and computer and compare.

[txcncman]

Might also be a way to start learning to read and understand G-code. I teach my students to manually write G-code with all methods before they learn CAM, so they already know what these things mean.

[cob]

ok I get what WEAR does. it inputs the g41 and g42 that way you can just adjust to make the part bigger or smaller.

I get what computer does bassically just input the right diameter cutter on your offsets and it will do all the compansation for you you just have to have the same tool in the machine as in your program.

but Control looks like it is almost the same as Wear it is inputting g41 and
g42.
so does that mean I can also adjust if the part is bigger or smaller?
the difference I found is that in CONTROL it will give the start and end points off every raduis and also it will input the raduis of my part. which is easier to understand.

My question with CONTROL is how is iT compansating? it will not post it in the post or does it know just by giving the start and end points and the exact radius?

hope this makes sence. because I dont get why would you want to use control when it is the same as wear.

bare with me .

[Joesph Jackman]

control requires you to enter the full radius of the cutter in the cnc control. control outputs numbers that match the part print. what control does is often called part print programing.

wear doesn't require you to enter the radius of the cutter in the cnc control. if your part is too big, in most cnc controls you enter a small negative number such as -.001 so the part will be to size. if your part is too small you often enter a positive number in the control like .001. wear outputs numbers that do not match the print as it includes the radius of the cutter in the part program.

[Superman]

"Computer"
- no comp in program
- tool must be same diameter as programmed in Mcam

"Control"
- allows the use of cutter comp ( G40/G41/G42 used )
- outputs the actual profile that goes along the side of the cutter when the TOOL RADIUS is placed in the D offset value in the CONTROL
- Mcam toolpath is along the side of the cutter
- lead in/out must be greater than 50% of the cutter diameter
- a D offset value less than the tool radius in the control will cut closer to your profile
- a D offset value greater than the tool radius in the control will cut further away from your profile ( leave material ON )

"Wear"
- allows the use of cutter comp ( G40/G41/G42 used )
- outputs the tool centre line of the nominated tool as the NC code
- Mcam toolpath is along the centre of the cutter
- normally ZERO is placed in the D offset in the control for a tool that is the same diameter as programmed
- lead in/out values must be greater than any value that you may need to place in the control to adjust the program path to get size, should always have a linear movement for comp to adjust along.
- a negative D offset value means the cutter will move closer to your profile
- a positve D offset will make the tool stay further away from the profile ( leave material ON )

"Off"
- no cutter comp in NC code
- usually for getting a cutter to follow on top of a chain ie a single facing pass, or engraving text ( lead in/out is OFF for engraving )

[nikolaiownz]

"Computer"
- no comp in program
- tool must be same diameter as programmed in Mcam

"Control"
- allows the use of cutter comp ( G40/G41/G42 used )
- outputs the actual profile that goes along the side of the cutter when the TOOL RADIUS is placed in the D offset value in the CONTROL
- Mcam toolpath is along the side of the cutter
- lead in/out must be greater than 50% of the cutter diameter
- a D offset value less than the tool radius in the control will cut closer to your profile
- a D offset value greater than the tool radius in the control will cut further away from your profile ( leave material ON )

"Wear"
- allows the use of cutter comp ( G40/G41/G42 used )
- outputs the tool centre line of the nominated tool as the NC code
- Mcam toolpath is along the centre of the cutter
- normally ZERO is placed in the D offset in the control for a tool that is the same diameter as programmed
- lead in/out values must be greater than any value that you may need to place in the control to adjust the program path to get size, should always have a linear movement for comp to adjust along.
- a negative D offset value means the cutter will move closer to your profile
- a positve D offset will make the tool stay further away from the profile ( leave material ON )

"Off"
- no cutter comp in NC code
- usually for getting a cutter to follow on top of a chain ie a single facing pass, or engraving text ( lead in/out is OFF for engraving )

Hey Superman

What do you use?

Ive always used Control since im used to it from when programming iso by hand.. but ive seen many use wear only but i dont like when i dont have the actual numbers in my drawing in my program..

If that makes any sense.

[Superman]

Hey Superman

What do you use?

Ive always used Control since im used to it from when programming iso by hand.. but ive seen many use wear only but i dont like when i dont have the actual numbers in my drawing in my program..

If that makes any sense.

Wear,
- comp in the control is always zero ( easy to see ), when correct diameter cutter is used, -- if a regrind then a negative comp would be input. I try to use a smaller tool than what is programmed if the correct size is not available. You tend to get errors if you try to go to a larger cutter

too easy to stuff up a part when using tool radius ( in Control ) if you forget to update the cutter rads in the control

you get to a stage where you don't actually read the NC file, run above the job to make sure Z depths & retracts are good, most problems are when starting each operation, or retracting / moving to the next op


- in the end, you are measuring the part to the drawing, not the NC file