MCam Mill/Turn... something doesn't add up for me

[jlw™]

Gentlemen,

 

Something isn't adding up for me in mill/turn.  I was expecting some magical software unlock but I've received a lathe machine def and post for my E1600 mill/turn.  No problem, I'm not worried about that - I've received excellent service from Postabillity.  They always come thru on my requests.

 

Preface:  I'm an Esprit guy until we made the switch to MCam.  Now there are a few things I want and the only thing I truly miss is the little box where I can type in a C angle and boom I got it.  In my milling machine defs (as you may have seen in a recent post) I initially had trouble forcing a C angle so I can reach where my head/table machine X axis travel limit is.  To do this in mcam, I create a plane that has X oriented to where I want it with the same Z vector as TOP.  Then just set that as WCS and TOPTOP as T/C planes.  Set offset and it works and posts out as desired.  It works beautifully in my mill defs.

 

Here's what's messing with me.  The lathe z = world z WCS is not like anything I've ever seen.  When I bring a part into the lathe def I can set WCS to top and orient the part as it physically is in the machine.  Then I switch back to lathe z = world z for WCS.  From there everything is good, created planes work out and all.

 

Here's the problem,  I can't for C axis angles because I can't wrap my head around where that lathe z WCS is at.  None of the axes match the physical realy world.  If I post with TOP as WCS B axis is the only thing that is correct but post with lathe z and everything is correct.

 

Now the problem is that I can not seem to find how to orient my planes to make a new WCS so that I can force C axis angles.

 

In the attached pictures, I have only changed the WCS.  Nothing was changed in the orientation of the part.  How do I go about creating planes to give me the desired C angle that I can use as WCS just like in my milling defs.  Or is there another way to force C angles in a lathe def?

 

Pic 1 WCS=TOP:

 

Pic 2 WCS= Lathe Z = World Z:

 

Any help wrapping my head around this mcam lathe def and why the WCS doesn't match the physical world would be GREATLY appreciated!

[Guest]

Technically, you're not running Mill/Turn

 

That is it's own product

 

What you are running is Mastercam lathe with a mill ability.....

 

To say it's quirky, that would be a minor understatement

 

I would say, start with your part at your known starting location and make and create planes as needed, don't pay a ton of attention to the MCAM WCS other than really as a starting point.

 

Try using the C Plane utility until you get the hang of lathe planes

 

For Lathe C planes they should always start as a rotation of the Back plane for the correct orientation on a lathe.

 

JM2C

 

 

You will also find some good inforamtion if you open a mill/turn post and read the notes

 

 

#TURN TOOLPATHS:

#Lathe canned cycles:

# Supports lathe canned turning cycles through Mastercam.  This post

# is configured to process them.

#

#MILL TOOLPATHS:

#Mill Layout:

# The term "Reference View" refers to the coordinate system associated

# with the Mill Top view (Alt-F9, the upper gnomon of the three displayed).

# Create the part drawing with the the axis of rotation along the X axis

# of the "Mill Reference View" with the face of the part toward the side

# view (Mill Reference View X plus direction).  The Y plus axis of the

# Mill Reference View indicates the position on the part of C zero

# (View number 3).  The right or left side view are the only legal views

# for face milling.  The view number 3 rotated about the X axis as a

# "single axis rotation" are the only legal views for cross milling

# except for axis substitution where the top view is required.

# Rotation around the part is positive in the CCW direction when viewed

# from the side view.

# (The Chook 'CVIEW' should be used for creating milling tool plane and

# construction plane selections, C axis toolpaths in lathe perform

# this function automatically).

#NOTICE: View number 3 always indicates the location for C zero.  Milling

#        with a turret below the centerline indicates C at 180 degrees.

#

#Mill canned cycles:

#Cylindrical interpolation, G107 canned cycle:

# Cylindrical interpolation is created with axis substitution only.

# Use the Caxis/C_axis Contour toolpath.  Create the geometry from

# view number 4 if the rotation of C axis is CCW.  This prevents producing

# a mirror image.  Wrapped and unwrapped geometry are broken and arcs are

# lost so it is better to create flattened geometry.  Set the parameters

# in Rotary Axis not to 'unroll' and set the correct diameter.

# Use View number 3 as the C0 location.  Set mi4 to activate!

#

#Polar interpolation, G112 canned cycle:

# Polar interpolation is active only for face cutting (Right or Left).

# Use the Caxis/Face Contour toolpath. All paths must start and end at

# the 'C0'location for output to be correct. Chain geometry and set

# mi4 to activate G112 mode!

#

#Axis substitution:

# View number 3 is the C zero location on the part and corresponds to the

# Y zero position of the "Mill Reference View".  Positions are wrapped

# from and to the diameter of the part as CCW for the Y positive direction.

# If geometry is drawn from View number 4 (Bottom), it is correct for the

# wrap/unwrap on the diameter.  The radius of the specified diameter is

# added to the Z position in the post.  The Y axis is the only axis to

# be converted with mill/turn.

#

#Simultaneous 4 Axis (11 gcode):

# Full 4 axis toolpaths can be generated from various toolpaths under the

# 'multi-axis' selection (i.e. Rotary 4 axis). All 5 axis paths are

# converted to 4 axis paths where only the angle about the rotation axis

# is resolved. Use View number 3 for the toolplane with all 'multi-axis'.

# 4 and 5 axis toolpaths are converted assuming cross machining only!

#

#Y axis output and machining over part center:

# Output Y axis motion by setting 'Rotary axis/Y axis' in the NC

# parameter page.  This requires a valid Axis Combination in your machine defintion.

# y_axis_mch is set from the axis combination.

# Set 'Rotary axis/Y axis' in a machine with no Y axis (y_axis_mch = 0)

# to force linear/circular position moves in the XZ plane (g18).

# This allows machining over the part center.

#Caution: The machining must stay in the XZ plane at a Y fixed value

# when y_axis_mch = zero because no C (other than the Tplane) or

# Y positions are output!!!  This occurs when selecting C_axis/Cross

# Contour without 'y_axis_mch'.  Use Mill toolpaths for cross profiling.

#

#NOTICE: Milling through the part center with a linear move requires the

#        geometry be broken at the centerline.  Milling through the part

#        center with an arc move in the G18 plane, no Y axis and on the

#        negative side of X, reverses only the arc direction and I sign.

#

[jlw™]

Thank you JParis, having read your posts and seeing the level at which you perform it makes me feel better to hear you say "quirky at best."

 

I did as you said and disregarded the lathe wcs just like when I orient my part.  I then went back to wcs = lathe and used dynamic planes to rotate it 180 so I could set that as my new wcs to force C to 180.  It looks good on the screen just as in milling but then it posts C90. which is absolutly fumbuzzling me.  I took the wcs that posts correctly as is but then spun it 180 thinking I "should" get a C180 move... nope, C90.

 

I guess like you suggested, I couldn't care less what the wcs gnomon looks like as long as I can understand it and get the output I want.  I don't care what it looks like.  I just want to know how to get my post to work like in milling so that I can get results every time with out playing around.

 

The sample lathe part I received from my post vender is too simple.  Would you be willing to send me a more complicated part so I can dig in?

 

Side note before every one suggests it:  I have been to training at CCS for all the milling topics and I'm kicking names and taking butt with mcam mill.  Having said that I will get Lathe training when I can but with my work load and the 2 new machines and a ton of major jobs I just can't get away for classes right now.  I'll have to wing it till then and hope that the forum can give me a little help along the way.  And I have the lathe tutorial but it is very limited on plane work.

[BenK]

Jlw, Can you send a z2g file? I would have time to look at it later tonight. 

[jlw™]

Nah, proprietary. But I'll gladly make a sample file to share. Any one who wants it will have to get it by email - I'm out-o-space on emc and it won't let me delete.

[jlw™]

That info is not in my post, which one is that JParis?

[Guest]

That's from one of the Mastercam 4 axis generics 

 

Generic Fanuc 4X MT_Lathe

[jlw™]

Cool, I'll dig in asap.

 

I am very grateful for you guys helping and being willing to help!

[Guest]

 

 

Would you be willing to send me a more complicated part so I can dig in?

 

If you can shoot me something in a z2g file, I'll be happy to set up a few things for you...

 

Unfortunately all of the stuff I do is covered on NDA's and sending out is something I can't do with customer files  

 

jmparis65 at gmail dot com

[The Cathedral]

Part orientation and WCS in lathe is nothing like mill. Looking at your first picture, you have your part oriented the wrong way. It's dumb, but when you draw a part in lathe, it's as if you're looking into the machine, instead of like mill where you're looking down the spindle. See the picture below.

 

You should have your part oriented so actual lathe z = mastercam x, actual lathe x = mastercam y. In order to look "top down" on the part like you do in mill, you would have to use the "right wcs" view.

 

C0 is the mastercam y axis. I never use anything other than the default  "top" wcs when I'm starting a job; using the lathe z = world z and other things is just too confusing and never seems to work right for me.

 

[Mike-T]

Like Cathedrals pic.. the bores will be be along the x axis in the top wcs and view. I use several of Dave's posts. your top pic, I would rotate the part so that the flat on the

od was at 3:00 oclock in the right view.. this would be B90C0. View back would be B0C0. , flat towards you. And like he said.. wcs always top, I make a copy of Top wcs for the subspindle.. same part orientation but origin moved by length of part.

[jlw™]

I've wrapped my head around the part orientation, actually pics 1 and 2 of mine are correct but illustrate the difference in mill and lathe. It's a VTL. I just don't get why Z in the physical world is X in the mcam world. Thanks to BenK and JParis I've let go of common sense and figured out how to force C angles so I can get around X axis travel limits.

 

I just don't like the mcam world not matching the physical world. It makes setting up new planes a bit slower but the more I do it the better that'll be. My machine def also has a "named plane" that is "Top" and if I select it the XYZ gnomon is correct to the real world.

 

Just going to take some getting used to.

 

Since your running a Postability post, how are you handling inclined plane machining? Are you using G68 or G68.2 and G53.1? I've got to have a few tweaks and I've always used 68.2 so that the control will handle deviation from COR.

 

How are you doing it?

[YoDoug®]

Gentlemen,

 

Something isn't adding up ...........................................................................................E1600 mill/turn.  

Preface:  I'm an Esprit guy until we made the switch to MCam.  

 

I want to know what Mcam salesman was able to go into a shop with an E1600 and convince them to dump Esprit and switch to Mcam. That guy could sell snowblowers in hell !!!

[Watcher]

Two things comes to my mind :

 

The shop wanted to reduce costs with maintenance.

They wanted a CAM with slightly better CAD capabilities.

[jlw™]

We got a new plant manager. His call to make the change.

[crazy^millman]

Guys here is my thoughts as I and our group have used the MT product in some very high profile companies. MT has come a very long way in a short amount of time. It does have some room to grow, but people have been putting a lot of hard work to make it a good product. Mastercam can program just about any machine out there, maybe not to some people's liking, but nothing can be everything to everyone. The product is right where I said and thought it would be. It is getting the attention it needs granted not as much as I or others would like, but I can personally say it is getting attention and focus.

 

jlw I Mastercam will program that machine, but I would get away from programming it like a VTL and program it like a regular lathe. Take a little bit to wrap your brain around the idea you are programming a vertical machine horizontally. Once you do and see how you can control everything and make some really amazing toolpaths to run these types of machines just the way you want then you see where Mastercam can get the job done. I was programming Integrex machines back in 2007 with Mastercam Lathe/Mill well before we had the MT product and have had my share of complaints. I like others want to see better stick machine support and generic Fanuc support, but I see it coming.

 

I have been programming 2 Turret and 3 Turret machine with Mastercam. I have taught a few people how they can also use Mastercam to program these types of Machines. Is it perfect, nope. Can it get the job done and allow you to get the machine running yes. Things are much better than they were many years ago. I give it another few years and it will be a very solid product.

[jlw™]

5AC, 

 

Thank you for the input.  I have no doubts mcam will do it... I'm wearing it out with it once I fanally wrapped my head around the wacky WCS/Planes.  We're several jobs into it now.  I've almost got my post tweaked too.  At this point I want some changes but I can post and run with ZERO hand edits so I'm good there.

 

Just took me a minute to finger out the planes.  MCam lathe is a bit different than I'm used to but it's doing the job and I'm excited to try out the dynamic turning soon.

 

Mcam can program any machine in my opinion too, I'm kicking tail on our 6 axis Vtech with it.  It just takes a little effort to calculate W positions to poke into a MR but I'm pleased with the output and the programming style.

 

Thanks again gentlemen!

[Mick]

Two things comes to my mind : The shop wanted to reduce costs with maintenance. They wanted a CAM with slightly better CAD capabilities.

 

Yes, regardless about what some others would say, it certainly wouldn't be for Mill/Turn capability

 

I agree with JParis, Mastercam Lathe with Milling is indeed quirky.

[mikenaturalice]

Part orientation and WCS in lathe is nothing like mill. Looking at your first picture, you have your part oriented the wrong way. It's dumb, but when you draw a part in lathe, it's as if you're looking into the machine, instead of like mill where you're looking down the spindle. See the picture below.

 

You should have your part oriented so actual lathe z = mastercam x, actual lathe x = mastercam y. In order to look "top down" on the part like you do in mill, you would have to use the "right wcs" view.

 

C0 is the mastercam y axis. I never use anything other than the default  "top" wcs when I'm starting a job; using the lathe z = world z and other things is just too confusing and never seems to work right for me.

 

Untitled.jpg

Looking at your picture, isn't that how you are supposed to do it? I have always done my lathe stuff like that. I think of it as looking into the machine with the part chucked, so the "top" of part is actually the od. Just a random thought I guess....

[crazy^millman]

Looking at your picture, isn't that how you are supposed to do it? I have always done my lathe stuff like that. I think of it as looking into the machine with the part chucked, so the "top" of part is actually the od. Just a random thought I guess....

 

Mike is all about prospective. I am left Handed and for most Right Handed people the way I look at things make no sense to them. I can see it most times from a right hand prospective because the Machining/Manufacturing world is approached from a right hand prospective. Flip it around and think about writing and using the opposite hand you normally use? I have become ambidextrous over the years being a machinist and programmer. Most controls on on the right side of the machine, all machinist tools are for right handed people and a left handed person drags their hands over what they write if they don't write inverted. Prospective is a power thing and wrapping your brain around someone else's prospective is sometimes more work than the project you are working on. 

[The Cathedral]

Looking at your picture, isn't that how you are supposed to do it? I have always done my lathe stuff like that. I think of it as looking into the machine with the part chucked, so the "top" of part is actually the od. Just a random thought I guess....

 

I guess I'm confused on what your asking. If you're asking if the way I do it is the way it's supposed to be done, well, I'd like to agree with you...

[BenK]

Looking at your picture, isn't that how you are supposed to do it? I have always done my lathe stuff like that. I think of it as looking into the machine with the part chucked, so the "top" of part is actually the od. Just a random thought I guess....

 

In all reality both are correct. You can either have your part vertical (along z) or horizontal (along X). You would just need to setup your planes appropriately for whatever method you choose. I have done both but horizontal does seem to be easier so that is how I choose to do it.