5-axis clearance move

[TheePres]

Need some advice on how you 5-axis gurus handle adding a clearance move to a 5-axis program.

Drilling at 1 end of large radius, then i would like tool to swing about radius to position for holes at opposite end. I was playing around with 5axis curve some,is this the method to use or is there a better way?

File is in X3 folder 5axis-clearance.mcx.

[Greg Williams]

I add a misc interger flag to the post to retract the Z axis to a given position at index

[crazy^millman]

Well no guru here. I handle this a couple different ways really depends on the toolpath I am using as well as the type of 5 axis machine I am programming. If I am doing a simple 5 axis drilling toolpaths on a head machine then I will use the point toolpath approach. I will make a c-plane at the index angle I am looking at for my head. I then will make a rapid point approach and retract since the drilling toolpath does not have the same parameters other toolpaths do. I will also use the drill point toolpath for 5 axis operations when I want to control the approach and retract to a certain place. Now if it some heavy head movments and I am not sure what Mastercam is going to do going from one place to the next and I do not want to go home to know I am safe then I will back plot the toolpath. Save it to a Level and then use the curve 5 axis approach when I make a line my vector then use a 3d line as my drive chain and then an end Vector. I have gone as far to have 20 tilts along a curve to keep the head close to the part bu clear clamps, stops, and raised bosses on the part. When you are programming big machines things like this really help the green to green time. I have seen some guys always send the head home then index then come back to me a complete waste of time. Does it take more work planning and programming all of those types of paths well of course, but that is what separates the people who care from those just collecting a check.

 

Now if it is a Trunnion machine most times I pick a safe height and send the machine there then index and do the work since almost every trunnion machine I have ever seen is no bigger than 30" of Z travel. The extra seconds it take to clear the spindle really makes no difference verse the risk of crashing the machine.

 

I guess the bottom line is Mastercam is really lacking when it comes to knowing what the machine will do when programming 5 axis. I really feel bad for guys that are in the same boat as me programming 5 axis machines with no verification software of the NC code. Mastercam has lacked in this area for years and I remember when X came out was only a matter of time and we where going to see full machine simulation well been what 5 years since we 1st started testing X and still no machine verification brought to you by Mastercam.

 

Do not get me wrong I like programming in Mastercam, but way to many wild arse promises made that have never come and in 5axis land that costs time and time is money and for people who can not convince management a $20k to $60k verification package is the answer we are stuck trudging our ways through making good programs with no real way to see problems on the machine until most times it is too late unless we are programming it like mentioned above know where at all time the tool is in relation to the part even doing what should be normal things like take the tool from one side of the part to other.

 

Just my take on this whole thing for what it is worth.

[TheePres]

Im with you Crazy Mill-Man,

I have been sending a few 5-axis programs out to shop now and feel that sending home for clearance stuff a bunch of bull, its lazy and a cop out.

I want my toolpaths to hug the part on positioning moves and love to have the operators sweat it some and keep back end muscles tightened while setting up my jobs.

The Catia programmers here use VeriCut software, but they are of no assistance in helping me intergrate this into MasterCam. Could you tell me if Vericut works with MC or only with final G-Code?

[gcode]

quote:

---

Vericut works with MC or only with final G-Code

---

Vericut has a chook that will launch VC from inside MC.. you can set it to run NCI or gcode..

 

I like the 5X curve method for motion between cuts, but it can be a lot of work.

I'm using the advanced 5X stuff more and more

There is a lot of power and control available to you on the linking page.

[Steve Hattori]

+1 on the adv 5x and its positioning control- the linking page gets it done where mcam fails.

[JohnW@Kauffman]

Most of my stuff is production trimming or drilling plastic parts. Agree with the control that the adv. 5 axis paths gives on the linking page, and I've used 5 ax curve for transitional moves as well. When I use 5 ax curve, I'll use offset contour to set up the curve I want the tool to follow from the part geometry, then set a high feed rate for the transition. I proof run all the parts before the operator ever sees them in production.

 

It is fun to watch the operator tighten up a bit when he sees the tool moving that close to the part for the first time.

[j.nguyen]

Hey G-code

 

quote:

"Vericut has a chook that will launch VC from inside MC.. you can set it to run NCI or gcode.."

 

I know mastercam can directly run the NCI file

though Mastercam but didn't know there was a C-hook to directly run G-code with out defining your tools or your translation matrix. Where can I find this C-hook? I really don't want to run the NCI because it doesn't show all the rapid moves correctly, rotation moves, etc. This would be helpfull thanks in advance.

 

Jamey

[gcode]

a copy of this chook is installed in the

Vericut folder on your computer, but you'll probably need to get the latest version from your dealer

I've never used it to run gcode, but I think

all it would really do is semi automate the setup process you go through for a regular vericut session.

It will create a tool libary from your Mastercam

library, ask you for stock and design models and

place them in Vericut space.

You'll still need a valid Vericut machine and a control definition.

 

While we're on the subject of Vericut.

I got an email from my dealer Friday..

Vericut 7.0 will be out soon.

[j.nguyen]

Gcode-

 

I will do some research and see how that works. Maybe Ver. 7 will not give you that out of memory err when working on large files even after changing you cut tol.

 

Thanks!

Jamey

[gcode]

quote:

---

I will do some research and see how that works. Maybe Ver. 7 will not give you that out of memory err when working on large files even after changing you cut tol.

---

If you are running files so big it brings Vericut to its knees, get an x64 computer..

I have XP x32 at work.

I used to run XP x64 at home.

The difference was night and day..

Vericut is x64 compliant. Get an x64 computer

with 8 gig of ram.. Vericut will use it

[jean]

Great feedback, thanks guys..

[gcode]

On ‎8‎/‎30‎/‎2009 at 2:57 PM, gcode said:

Get an x64 computer

with 8 gig of ram.. Vericut will use it

a blast from the past LOL

Amazing how much our computers have advanced.

32g is mainstream for a Cad/Cam PC now.. power users run with 128g

 

 

[crazy^millman]

Yes blast from the past now I have programmed Trunnion machines that are 1000mm and some 5 Axis machines that have 220 foot of travel. We have machinesim now and that has helped our programming efforts. Still programming in Mastercam and still earning a living doing so.

[Aaron Eberhard]

I was just wondering who could afford 8 whole gigs of RAM!

 

Madness!  

[cncappsjames]

That's a SERIOUS blast from the past. 

 

[TheePres]

Oh wow, this does go back a bit. Thanks to advice and assistance from you great guys, that's all I work on now is 5 axis work.  Though plenty of time,  I do miss a "gravy" part.