[badRandle]

When I try to contour a .5 hole with a .25 endmill using control comp. climb milling, the lead in - out goes outside the .5 hole boundary. How do I get the dia. comp to follow the lead in-out??

Confused *&^($@

ThanX
Randle

[cadcam]

Well have you tried a smaller distance for the lead in lead out.
Also if you want cutter comp being G41 or G42 you will need to change it to Wear if you are running MC9 or higher.

if you are using 9.1 you can get the tool to comp before entrying the hole if you want say at the rapid plane.

Now did you want it to helix in to the hole following the profile?

[badRandle]

Thanks for the reply.

I am using 9.1, just loaded it a few days ago.

The problem I am haveing is this: I just started a new job where all the CNC operators are and have been using radius comp toolpaths, where they add in the radius of the actual tool in the tool offset register on the machine, so the toolpath is the actual line of the part. Since they already have hundreds of programs written this way I am try to keep them the same.

My last job I programmed all toopaths with computer or wear comp. and the only offsets were the difference in real and net size of the tool used, or small adjustments.

I have gotten MasterCam to program contours in control comp, the only problem is that I cannot get the comp started before the lead in-out, so the tool goes down to the start of the lead in, moves to comp and then follows the lead in toolpath. If I could just get the tool to start off the part (outside profile), arc into comp, go aroung the part, overlap and the arc away out of comp that would be ideal.

The other option is to program with wear comp and teach the operators to set-up with zero tool comp. Some of the oldtimers are most likely going to forget at some point and see a zero comp and add in the raduis like they have been doing for years and then CRASH!.

Thanks for your help.
Randle

[hardmill]

OK bad,
If you can't change the way they do things just add a little
geometry (line perp. to entry entity),so your comp. turns on
before making contact w/ your workpiece. Just a thought!
I can't answer you till I try it for myself. I'll post again on
Monday, if Jay don't beat me to it.

Jay are you there?????

[Andy]

Choose:
Comp in computer OFF
Comp in control LEFT
Choose the chain direction correctly for inside or outside contour.
Choose a reasonable Lead in out.

Should work fine whether your contouring inside a hole or outside a contour. Vary the lead inout to fine tune.

Andy

ps At least in V8.11 it works.

[hardmill]

Welcome to the forum.
I take it your a MasterCam user?
How long have you been a MC user?

Great to have you here.

[CAMmando]

What andy said +

On lead in, use line and radius. Make sure the line length is greater than 1/2 the anticipated cutter diameter in order to properly apply comp.

Use the overlap parameter to cut past the profile start prior to leadout.

Seriously consider talking to the men about moving to WEAR COMP as a standard. I know its tough because the numbers wont match the print, but I have found that inevitably you wind up with comp more errors and reprogramming when programming to part geometry. Especially on complex part s.

As far as mistakes, you can add logic to your post that checks for the type of comp and posts a comment:

(*** WEAR COMP ONLY - DO NOT ENTER TOOL RADIUS ***)

That should be clear enough.

HTH

[Rekd]

CAM, you're really starting to scare me...

badrandle..

Make sure the line length is greater than 1/2 the anticipated cutter diameter in order to properly apply comp

This should fix all the problems that CAN be fixed when using this type of CRC.

IMO, and from my 15-20ish years as a CNC guy, I've used them all. CAM is right, again, in that you will have problems of one sort or another using your current method. Yes, it's easier to check the moves in the program, but is it worth it? Not in my opinion. There's lots of room for errors and that's money.

Your guys need to learn to work in the 21st century. That's old school, and it's old for a reason. There's better more reliable ways to do it.

'Rekd

[CAMmando]

CAM, you're really starting to scare me...

Why's that ... something I said or the new avatar ?

(dark)

[SRT]

I've been reading the MC forum here, with the hope of one day being able to purchase that software. You all have been discussing a topic that I'm not familiar with (Control Comp. & Wear Comp.). As I'm trying to follow along, are you saying that as an example: in control comp. you would set the offset at the machine as .500-->.505, and in comparison, in wear comp. you would set the desired correction to .005 at the offset in the machine? Is this a unique MC process or is this possible in other software also.
Thank You.

[CAMmando]

Hi SRT,

* None- M/C programs the tool c/l on the tool path geometry.

* Control - Comp in control: M/C programs the tool c/l on the tool path geometry AND outputs COMP CODES (G41 or G42).
- So you input 1/2 the end mill diameter into the machine control comp register.


* Computer - Comp in Computer: M/C programs the tool c/l offset from the toolpath geometry by 1/2 of the programmed tool diameter.
- No comp is used in the control.


* Wear - Comp in Computer: M/C programs the tool c/l offset from the toolpath geometry by 1/2 of the programmed tool diameter AND outputs COMP CODES (G41 or G42).
- Comp is used in the control only to "fine tune" the size. The amount entered uin the machine control is only the difference between the programmed tool size and the actual tool size.


Hope that helps.

[cadcam]

Ok Randle, there is a new feture in MC that you can insert the cutter comp out side the cut may be this what you should use to make sur there is enough room every were.
But What I have to see is how it will work with "Control instead of "Wear".
I will be comeing back with more on this.

[hardmill]

Radius comp is pretty old school, not that many people use it
now that we have cadcam (noy you jay). Back in the day
it was easier to program(manually) the numbers on the
print than to figure out tool centerline. Then offsett 1/2
the tool dia. with your tool comp.

I know this stuff and it makes me feel old.
PEACE

[CAMmando]

One exception to this is Wire EDM where the control is comping wire offset based on power settings. In this application it is still common to program part priofile.

[abcdef]

use this formula
y = (dia of hole - dia of tool) / 2 * .4142

put y in length of line and arc radius ( NOT IN percentage column)...

135 Degrees in Sweep...

that's it and tool comes down right in center...
good luck..

[MnotLyon]

When I try to contour a .5 hole with a .25 endmill using control comp. climb milling, the lead in - out goes outside the .5 hole boundary. How do I get the dia. comp to follow the lead in-out??

Confused *&^($@

ThanX
Randle

On some controls you can turn cutter comp on, make your first straight line move, then move z into the hole. That won't work on older controls though.

In this case, I would use an entry exit arc of about .22 and 90 deg. Then, I would use an entry line of .22 that is perpendicular to the arc. That will cause you to drop into the hole pretty close to the center, and should give you enough room to turn on your comp for most controls.

[Mike Mattera]

Didn't read the whole thread but..... Sounds like Line, Arc will fix any comp errors your getting.

If your doing a hole, Put a point at the center and Pick the Point, Then pick the Arc (for the Contour). On the Lead In/Out page make sure you select Start from the Point & Finish at the Point. And of course Line & Arc lead on values.

Mike Mattera

[rapid]

i once had problems with this using a drill/chmf/threadmill tool.
our guys were used to using 0 for cdc offset or wear but i had to use full cdc.
i never had the thought at the time and it was a expensive tool so much that we switched to standard drill & tap.
all i needed to do was add a macro to check the limits of the offset and if out of range alarm.
hindsight i guess.

[chuy]

us circle mill toolpath always starts center of hole...if not here's a little formula to make it start center of hole everytime...Hole dia.- tools dia. / that by 2 x that by .4142 insert this # into the entry and arc with an angle of 135 deg works for whatever size hole....

[cadcam]

WOW Chuy tat is old MC9.0 not even V9.1 .

Hey for fun a gigles try this tell it to create virtical lines. now create say 35 just by sketing the what happens?