Mazak Integrex

[RStuart]

Looking for anyone with Version 9 and using a newer model Integrex. Have questions about some things including the post and generating 5-axis tool paths as well as the machines ability to run extremely long programs.

[chris m]

Sir,

 

As far as post processors go, there was a thread a couple of months ago in this forum called "Integrex posts" or something like that [started by me, actually] that generated a pretty good response. Unfortunately I am not slick enough with this web stuff to create a link to it, but I'm sure one of the other, brighter, guys can do it. We're still having problems getting our machine to pass our acceptance criteria so I don't have any other help to offer at the moment; sorry

 

C

[RStuart]

Chris,

I saw the thread from a few months ago. We do have a post at this time, although I am having some problems getting it to generate 5-axis code. I have made parts with mastercam with great success, although I am still undertrained as far as MasterCam is concerned. I heard they (MasterCam) were putting together a class designed just for the Integrex machines. I have been running and programing ours for almost two years now and I love the machine. I thank you for you input and if I can help you or any other out there give me a shout.

[McRae]

Integrex... Dave has the medicine for your illness.

 

The Integrex is only capable of simultaneous 4 axis motions using the Fusion 640T. This I am told is changing as Mitsubishi is releasing the continuous 5ax technology to Mazak (Previuosly only available with a Fanuc Control). So my first observation would be that. What type of tool paths are you wanting to create and the second part of the equation, what types of tools do you intend to use. If using the machine for rotary type tool paths, watch the c-axis torque when you try to drive around the part, there may be a limit to how hard you push the machine. I suggest to rotate the c-axis, lock the spindle and then do some of the roughing, Index-Lock-Rough, then the c-axis will not limit performance.

 

With the turing of the parts - this is easily handled by the post - I have never had an issue.

 

Coolant options - have the post configured for this.

 

Spindle Speeds - Get the gear table setup right or the operator will scratch his head wondering why the machine sits still in the morning even though the M4 is telling you it should be running.

 

This is important. Mill and Turn INTO the ways of the machine (ie - M4...) This keeps pressure on the y-axis and therefore reduces vibration.

 

Never, Never, Never try to cut corners and order Mazak VDI holders from anyone but the OEM, Pay the extra and get the right stuff once.

 

There is no CAD/CAM system or company activly developing tool paths to work with the Integrex, I have had extensive consultations with their Applications Engineers in Kentucky and we share this observation. The nature of the tool paths tha you can create are only limited by the users knowledge of Mathematics and Vector Mechanics. Get used to the phrase "No one has ever needed to do that before..."

 

Watch out as the new E Machines are really cool and don't get me started about the "Vertigrex"

 

Max File Size:

There are a few options here, but in order to run from memmory where you can see, touch and feel all the g-code it is 1.02Mb. You are capable of running off the Hard Drive where the file can be stored locally on the machine's own hard drive or map a network drive and run it from there. No fancy DNC required for this - It just does it on its own. So file size is not limited at all.

 

[ 08-27-2002, 12:56 PM: Message edited by: MfgEng ]

[RStuart]

I am trying to machine a relatively simple yet semi-large part, mainly consisting of four angled flat planes. All I want to do is generte a finish tool path manipulating the B-axis to the desired angle, then using the X,Y,& Z axis to machine the flat as smooth as possible. I am doing all of my roughing using the X,C,& Z axis. Surface finish is my goal. As of now I am using a surface finish contour with a very small step down with a ball end mill. The finish is o.k., but could achieve better, & faster if I could do like I said above. I think maybe my problem stems from one of a few thing. Lack of experience on MasterCam. I have only been working with it for about 8 months, but have made a couple pretty complicate parts on it. I think maybe the axis limitations in the Y axis may pose a problem. One machine has 4.12" and the other has 4.56". My part is 13.3" in diameter. Although if you take into consideration I would like to use a 2 or 3" face mill I am not lacking much. But I cannot even get it to generate partially. It draws it fine,but the code is incorect. Which brings me to my final thought. It could be a post problem. Also as far as the memory in the machine goes, we have both of our integrex's network through a p.c. and I have no problem getting the programs to the machine. Although with this particular program it tends to lock up the control when I try to bring it up on the program screen. A sof now the program generates almost 13,000 lines of code. Another problem that I am having concerning MasterCam is that it takes alot of time to post this particular program, around 30 to 45 minute. I have 128MB of RAM and have roughly 100MB alocated for MasterCam...... Any suggestions on all I have said would be greatly appreciated....

[Guest CNC Apps Guy 1]

quote:

---

I have 128MB of RAM and have roughly 100MB alocated for MasterCam...... Any suggestions on all I have said would be greatly appreciated....

---

That is WAY too much allocated to Mastercam. You NEED AT LEAST 32MB for Win98 and NT 4.0 to run properly, 64MB For Win2k Pro, and 128MB for XP Pro. Mind you these numbers are for the OS ONLY. Adjust your MC Allocations accordingly. If you've got Win2k or XP, I'd run down to the computer store and pick up another stick or two of memory. It's so cheap now that to have less than 256MB really does not make sense.

[Michael Reynolds]

Hi RStuart!

 

I'm from Corning Community College, which is in your neck of the woods. If you need any of your programming staff trained, please let me know!!!

 

(shameless marketing, I know......)

 

Mike R.

[Guest CNC Apps Guy 1]

Tsk, Tsk, Tsk. Mike.......

 

Nice touch. I'll have to use some tact next time I'm pimping my expertise for $$$.

[Fred from Université de Sherbrooke]

Rstuart,

Are you using the G124 macro? With this, you can create a toolplane in Mastercam, and the B axis will be tilted perpendicular to your plane.

Hope it help.

[Rich Taft from CNC Software]

RStuart,

Mastercam Lathe offers you a choice of Y axis, C-Axis or Axis Substitution in the Rotary Axis Dialog on the parameter page. This parameter is set at the operation level and is active for the entire operation.

 

As far as posting speed, if you turn on Y-Axis in the BEADFEEDER.MC9 file you can expect to post in about 1/10 of the time because we don't have to break up your toolpath into XC motion.

 

I hope this helps.

[Michael Reynolds]

Hi James!

 

Who said I'd charge them????????????

Respectfully,

 

Mike R.

Shameless MasterCAM Perpheser

[RStuart]

Mr.Taft,

Thanks for your help and the email you sent me. I am sure I will be calling on you here in the near future, if I haven't already. Although, what you suggested about using the Y-axis is not going to work for me. Unfortunately the part is too large for the use of the Y-axis. The part is 13.189" in diameter, and I only have a Y-axis travel of plus and minus 4.12" on one machine and plus or minus 4.56" on the other. Is there a way that I can manipulate all axis' to remedy this problem that the integrex is capable of doing. I am start to realize that when Mazak calls the Integrex a 5-axis machine, its more or less a half truth! Any how, I am having some problems with my post and I will get in touch with you soon to try and sort them out. Thank you again.

[Rich Taft from CNC Software]

RStuart,

Thanks for the email. I'll take a look at your B-Axis idea to see if we can get a path within machine axis limits that way.

 

One other option that can be helpful in cases like this is the G12.1 (G112) machine cycle. You can program Y-Axis output in Mastercam and turn on this cycle via the Misc. Integers and the machine will do a polar conversion. It is typically tied to Misc. Integer two or four depending on what version of the post you are using.

[Guest CNC Apps Guy 1]

RStuart and Rich,

 

True the machine has ± 4.12 or ± 4.56, but isn't that is assuming that you are starting from centerline? Don't you have more + if you're starting from below centerline?

[McRae]

James is correct. The Y axis is a synthesis of the X and also the Yt Axis giving the Y axis as 30 degrees inclinded from vertical (Perpendicular to Slant Bed). When at X Reference position, We have less travel as X is close to upper limit travel. E-Machines will have unprecidented 30" Y-Travel!

[Guest CNC Apps Guy 1]

quote:

---

30" Y-Travel!

---

 

Holy cow that's some travel!!!!

[RStuart]

Unfortunately guys on our Integrex 400Y amd our Integrex 400IIY that is the travel at its max. As described the the machine specifications. Although Jim and I figured a way around that. Thank you everyone for your help. Greatly appreciated.

[RStuart]

Rich not Jim, sorry for the mix up.

[McRae]

What was the solution? We are dying to find out!