Lathe only c-axis contour

[DavidB]

I can't believe Mastercams full version of Lathe can't do Y-axis machinig.

Therefore if I had a shop with only Lathe machines, with Y-axis capabilities. I would have to purchase Mastercam Lathe AND Mill?

 

Also would I have to pay Maintanence on Lathe and Mill????????????????

[gcode]

quote:

---

What you are saying is a Y-axis toolpath can only be done with a MILLING toolpath

---

That was the only way I could get the Y axis

to output. Maybe someone else knows a different way.

 

At the very least you need a copy of Mill Level 1

added to your lathe seat. My dealer knew this

right away. I won't comment on your dealer as

that would probably be a TOS violation

[DavidB]

Well,

Today I finally got an answer from my reseller.

I have to purchase Mill leve1 1 as an addon for my Lathe only seat to be able to do Y-axis machining.

I also have to pay Maintenance for the Mill addon on top of the Lathe maintenance I already paid???????????

 

[Threept82]

DavidB

If your planing on intricate milling on your lathe then yes I would get mill 1. If your only planning on simple milling and holes I would do it by hand because it is simple to do if you know manual miull programming. X is the same as milling, Double the Y coordinate and change the letter from Y to C.

[Threept82]

DavidB

I didn't see the beginning of this tread. Seems You know what to do your just unhappy about the mill seat and Maintenance. Don't blame you I would be too.

Hey look up. Looks Like my sharks and diver are competing in synchronized swimming

[Glenn Bouman]

We sell lots of lathe only Mastercam to clients that do Y-axis milling on a lathe.

 

Maybe it is a northern hemisphere thing.

 

Watch the video.

[DavidB]

Glenn,

What you did on the vidoe we can achieve,but you can't machine a slot running parrellel with the Z-axis thats not on the centre line.Or drill a cross hole thats not going through the part on the centre line.

 

With a Lathe only seat of MC cross hole drilling that's not on the centre line eg:Lock wire holes,or grooves running in Spindle axis that are NOT on centre line can not be programed.

A milling level 1 addon is needed.

 

 

Gleen on your Video I noticed you have Cimco V5 where is this available from?I currently have V 4.32?Thanks for your effort in replying

 

[ 06-07-2005, 06:21 PM: Message edited by: DavidB ]

[Glenn Bouman]

Use Cross ctr.

 

example

 

Regarding Cimco V5, check with Anthony Graves, he said a Mastercam OEM of Cimco V5 will be available when X is released.

 

[ 06-08-2005, 07:17 AM: Message edited by: Glenn Bouman ]

[DavidB]

Glenn,

 

Thank you so much.

My MC reseller came into today to install the Mill addon.I showed him your Video Cross ctr.

He couldn't believe what he was seeing.

It was a post issue all along and the Mill addon is not required.So you have saved us $.

 

I owe you a beer or two mate thanks

[tryon]

what was it in the post if i might ask?

[DavidB]

We have Okumas so we are using the Okuma post's. Would you believe all it was a Misc switch.

And they wanted us to by a Mill addon

[crazy^millman]

Very very imformative thread. I am glad it all worked out for you David.

[DavidB]

Glenn,

 

Got the Cross ctr working great.

But how do you get a cross hole thats not on centre line working?

It keeps rotating the point so it's going from the drilling point through the centre.

Do you have to make a T/plane for cross drilling?

[DavidB]

Yippy,

I worked it out if you use an arc not a point as geom for drilling it using the arc to set Rotation.

[crazy^millman]

Just like 5 axis David can have a surface or face of a soild or 2 lines or an arc to set a cplane so good to nkow this if I get in the place were I need to program a y axis lathe.

[Glenn Bouman]

quote:

---

Do you have to make a T/plane for cross drilling?

---

Yes, if you set the tplane in the C-axis drl toolpath you will get y axis output. video

 

I think you have covered the limits of what can be done with a Lathe only system and Y output.

[DavidB]

Glenn,

If you create an arc where the drilling point is then select the arc as the drilling entity.MC creates the toolpath using the arc to set the T/plane.

Thanks for your wonderful help