Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

What angle do you use in Lead In/Out the most?


crazy^millman
 Share

What angle do you use in Lead In/Out the most?  

30 members have voted

  1. 1. Percentage used?



Recommended Posts

Okay I normally never use 90 degree to for my lead in and lead out angles. I go a little as 5%, but like to stay around 90%. My thinking is this for why I approach it this way. I never claim to be the expert, but logically have developed this process over the years and was thinking CNC could improve this by changing the default of 90 deg to maybe down to 30%. I would also love to see a slider bar to adjust these thing. Right now you have to adjust by manually typing the number. i would love to see a slider bar for these things in Lead In/Out verses the 25 year old way of having to always type the values.

#1 Reason the reduce the amount to travel which reduces the time to manufacture the part.

 

#2 Most newer machines do not need to Ramp up and Ramp Down curve to cut effectively any more. I am cutting at 450 to 800 imp on machines and with accel and deccel abilities we do not need the same room.

 

#3 I just like the way it looks. :turned:

Link to comment
Share on other sites

I use 2 different strategies, one for inside/pocket and another for outsude.

 

Inside, depending on the size, I generally like to start near the center of the hole . SOmetimes it'll be 5% line, 5% arc then 135 Deg is my angle, plus some overlap. That's my normal strategy.

 

In external stuff, I like to come in tangent on a corner at the srart of the entity, then sweep off 180deg a small amount baclk close to the start point, and keep tool down.

 

As always, this is subject to change based on part geometry/configuratino.

Link to comment
Share on other sites
Guest MTB Technical Services

Ron,

 

I'm a bit confused.

The angular sweep in the Lead-in/Lead-Out settings isn't defined as a percentage.

 

That said, if the contour I'm engaging is a closed internal contour,  I'll always ramp(not helix) into the part with an arc.

If it has CRC then I'll always use a perpendicular entry to a tangent arc for properly engaged CRC.

This provides three benefits.

 

1) Rolling into a cut ALWAYS extends the life of the tool.

2) You eliminate the possibility of a witness mark.

3) It works on every CNC control on the market today.

While some do allow engaging CRC with an arc, I never do that.

 

I usually set the angular sweep to 22.5 degrees for Lead-in/Lead-Out

 

For the purposes of CRC, especially on a FANUC type control syntax,

you must engage with a linear move and that move should never be tangent to the part geometry.

If it is, it must be at least as long as the max amount of comp being engaged or you'll gouge.

Even so, I would never recommend that method.

  • Like 1
Link to comment
Share on other sites

Small holes, I like to start in the centre. I used to use the chain and point, but I hate adding the point chain.

 

I used my little formula: (Diameter of Hole - Diameter of Cutter)/4 = Entry/Exit Arc value. Set Angle to 180 degrees, and it starts and finishes at the centre of the hole.

 

If ramping a helix, I only use the exit option.

 

For all other contours, it is usually 45 degrees, with a radius of what I think feels about right :)

 

I'd rather CNC work on improving other things. Entry and exit works fine. :)

Link to comment
Share on other sites

Small holes, I like to start in the centre. I used to use the chain and point, but I hate adding the point chain

I use Circle Mill for this.. driven by circles, not points.. that way geometry drives the size of the circle,

not a typed in value on the parameters page.

 

An added advantage to this approach is that you can mill numerous circles of varying sizes with one tool path

  • Like 1
Link to comment
Share on other sites

Ron,

 

I'm a bit confused.

The angular sweep in the Lead-in/Lead-Out settings isn't defined as a percentage.

 

That said, if the contour I'm engaging is a closed internal contour,  I'll always ramp(not helix) into the part with an arc.

If it has CRC then I'll always use a perpendicular entry to a tangent arc for properly engaged CRC.

This provides three benefits.

 

1) Rolling into a cut ALWAYS extends the life of the tool.

2) You eliminate the possibility of a witness mark.

3) It works on every CNC control on the market today.

While some do allow engaging CRC with an arc, I never do that.

 

I usually set the angular sweep to 22.5 degrees for Lead-in/Lead-Out

 

For the purposes of CRC, especially on a FANUC type control syntax,

you must engage with a linear move and that move should never be tangent to the part geometry.

If it is, it must be at least as long as the max amount of comp being engaged or you'll gouge.

Even so, I would never recommend that method.

 

Yes I worded it a little wrong, but I think what I was trying to get out of this will be okay.

Link to comment
Share on other sites

Well good conversation what I was looking for in this exercise. Thing it how many places do we have to go change that at in the defaults? We want a 30% default okay tell me an easy quick way to change them all to 30% or 15 degrees? Now I have 14 different default files for all the angles and all the percentages. Be nice to have an universal default place to set everything like this and be done with it. 30 different places use the same thing, but you have to go to each place and change it. No way I am ware of to say make default for contour toolpaths and have it carry all the way through for lead in and lead outs. If I am missing it then please point it out to me. I have a business to run and as I grow that business I need tools that save time not create extra work for myself or my employees. I am looking at this from a owners, programmers, operators, or any title you want to put in there perspective. I whip though all of this stuff at lighting speed. Trying to learn Mastercam looking over my shoulder not a pretty site. Ask few of the forum guys not that I am anyone special. Point is I see a place for major improvement in functionality and speed to get the job done. Making a strong enough case for that will hopefully make business sense to people who need to make these decisions. I am just a regular guy trying to earn a living like the rest of you. The easier my job is because of things that can be done better then the less hours I have to put into the work to get it done. I don't mind hard work, but if I can work smarter and have the tool that is part of that equation come along with me then I win and everyone else who is fighting the same time problems can benefit as well.

 

How many people even know about default files? How many have libraries saved with tools? How many people have template files to start with? How many people even take the time to define their holders for jobs? They claim they do not have the time. I can have 20 different default files, but how much is it going to take for me to set all of that up and then every version how much time will ti take to keep it correct? Sorry I want a one place stop and shop on some common settings for operations. Change it there get it done and call it a day. Give me that way and I figure I save 2 to maybe as much as 10 hours week on programming. I am one person figure that by 20,000 people using Mastercam I think I make a pretty good business case to really give it some consideration. Yes I know I am that same person I talk about not enough time to take out time and make all those different default files. Been there done that and will leave it at that. :geek:

  • Like 1
Link to comment
Share on other sites

I use Circle Mill for this.. driven by circles, not points.. that way geometry drives the size of the circle,

not a typed in value on the parameters page.

 

An added advantage to this approach is that you can mill numerous circles of varying sizes with one tool path

 

Yes, Circle Mill will do the centre point automatically, but wont to ramp down the bore, like when using Ramp Contour. Which is why I rarely use Circle Mill.

Link to comment
Share on other sites

Different settings for different applications.  Most common is a .050" tangent line with a .3125" radius 45° sweep for finishing peripheries with a 5/8 flat EM, two passes at nominal, enter and exit on first and last, keep tool down.  H13 at 46RC.

 

I keep my operations defaults library in my head, and by habit go through and set or check almost every field in an op.  I really want to develop operation defaults libraries and exported ops libraries for my SOPs, but I've been too busy keeping up with what needs to get to the floor.  I'm only on here right now because I'm regenerating a stock model.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...