Lead in / Lead out

[jcnewbie]

If I take a look into the lead in / lead out parameters there are many one could check and one could enter.

Is there a default value that I could put into these fields... Or is there more to it ?

[charger19690]

I guess I don't understand the question...

You can put any value in for lead in/out you want. Depends on what you want to put in there. I myself always put in something like .100" for in/out for a nice clean round number. If I have alot of stock, the number could be higher. If you use a Swept angle, it could be a completely separate number approach. In my opinion it comes down to the programmer and how much/type of movement you want/need for the particular part. (Talking about 2d contour pathes)

If you mean by 'default', you want a those numbers to be something of a standard for you each time you go in there it's "Pre-set", you can go in and Edit the Operation defaults in Mastercam.

If this isn't what you are asking, let me know.

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[Superman]

Your settings will alter constantly and will depend on how you run your machine
IMO
If you use "Control" for your cutter comp, then I would have defaults set to Tangent, 60% line length, sweep 90°, 100% arc radius.
60% because it must be greater than tool radius to take up comp

If you use "Wear" for your cutter comp, then I would have defaults set to Tangent, 25% line length, sweep 90°, 25% arc radius.

% is used as it is the only constant in this dialog area ( your tool dia is always changing ), so if you wonder why a number you put in alters, and you then alter the tool diam, it works on %

The figures will need to alter for each path, but at least comps would work, and you won't descend onto your contour, just watch out for other contours

[jcnewbie]

Thanks for the replies !


Why would one use Perpendicular and not Tangent in the lead in / lead out parameters.

As well should Gouge check be selected on all the time in the lead in / lead out parameter?

[thebowman]

Originally Posted by jcnewbie Thanks for the replies ! Why would one use Perpendicular and not Tangent in the lead in / lead out parameters.

Some possible reasons to use perpendicular rather than tangent:

You don't have enough machine travel.

The part geometry doesn't have the clearance needed to get on to the chain using tangent.

Some CNC controls require a straight line move that's at least half the radius of the cutter to turn cutter comp on and off.

There is a lot of power given to the user in Lead In / Lead Out.

If you haven't already check out Adjust Start Of Contour and Adjust End Of Contour. I use Adjust Start and Adjust End Of Contour all the time when putting a chamfer on a part to deburr the part. Much easier than screwing with the chained geometry so the deburr tool has clearance.

If you're new to Mastercam make sure you check out all the on-line resources for it.

[charger19690]

Originally Posted by jcnewbie Thanks for the replies ! Why would one use Perpendicular and not Tangent in the lead in / lead out parameters. As well should Gouge check be selected on all the time in the lead in / lead out parameter?

I personally use Perp lead in/out alot for programming for no better reason then it's alot easier to read the program and edit if need be.

If you use tangent with an arc, it's alot harder for operators/setup people to read the program and understand where it's going. (From my experience). When they are running a program and see a G41 line with a straight move, it's much easier for them to know where it's going and what it's doing.

I know I may get burned for this comment, but most of the shops I work at operators/setup people don't read programs very proficient, so making the programs as simple and standard as possible makes the world a better place......especially when they think they can make an edit here or there and put there fingers in the program.

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[Matt Berube]

Anytime they put their fingers in the program ONE SHOULD GET CHOPPED OFF !

No editing G-code allowed !

[Superman]

Originally Posted by Matt Berube Anytime they put their fingers in the program ONE SHOULD GET CHOPPED OFF ! No editing G-code allowed !

Be careful here,
I've had my a$$ pulled out of the sling by a good operator,
had the wrong WCS and all the NCfile needed was Z-depth alteration

The operators should be up-skilling their knowledge level as they do their job at the same time that programmers advance themselves
Why should we be the only ones to learn on the job, who is going to be the best choice to step into your shoes at the end of your working life.

The operators are a programmers best asset. Get them up to speed quick, as they'll help you more times than you help them.

[charger19690]

I kinda ride both sides.

I believe people should be empowered to fix things or change things "When needed" but if you don't know, "Please ask, I will explain it to you and teach you".

Besides, we all didn't know what we were doing at some point in our lives.

People always ask how I became a programmer, I say I didn't, just been faking it for about 10 years now....


Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[Matt Berube]

Superman & Charger,

I agree with both of you.

I have been saved many times by an operator who is paying attention.

I know that the structure and procedures of different shops vary quite a bit. Our place is pretty flexible and anybody that wants to learn about MC is encouraged to do so.

I am always willing to show anybody how to fix things in MC.

The point I was trying to make was that it should be fixed in MC and not in the NC file because we "back-up" MC files but not .nc files. If we edit the g-code then have to make a replacement in 6 months we'll run into the same issues all over again.

In our shop it makes much more sense to fix the MC file and re-post the program but I do understand that this strategy doesn't work everywhere.

[cadcam]

The lead in and Lead out are all about how you get the tool to encage with the Material.
Some time you don't have enough room to do a leaner move and an arc engagement in the area needed so being able to at least do a min of a line perpendicular.
All machines need at least a liner liner for cutter comp to be active; there are a few controls like older fadals that support an arc g02 or g03 movement.
Now with the lead in lead options you can turn cutter comp if needed above the part engagement and turn off the cutter comp again at the end above.

Another resin for the perpendicular option Example lets says you are trying to chamfer an edge that terminates at a wall so you want the tool to move along the drive contour as far as it can up to the wall before leaving the profile. So including an arc takes the tool away from the profile sooner, so use this option and go up to half the dia of the chamfer tool then move away.

Hope this helps