Mazak Integrex

[cncfrank]

Hey all: I've made a move...used to be just plain ole Frank. I've now got X, and have just purchased a post for a Integrex, and a 2 day on site training for X and this machine. Is anybody familiar with the integrex ? How good does it work with Mastercam ?

 

Thanks,

Frank

[chris m]

Try a search for 'Integrex' and you'll get some varying opinions about that!

 

C

[IntegrexMan]

Frank,

 

As long as you orient your part properly within MasterCam and your post is good, you will have no problems. Should you have any questions, feel free to let me know. I have been programming Integrex's for about 6 years. Did you get the machine with a sub-spindle, lower turret or both? If you have a sub-spindle, are you planning on running bar stock? If you need help with the transfer, let me know. The books Mazak gives you, don't explain it very well.

 

Craig

[cncfrank]

Thanks Craig ! I don't think we have a sub-spindle, and I know we don't have the lower turret. I'm just waiting for Axsys to provide a post and some training for it.

[IntegrexMan]

Well it should be very easy to program then, but if you need help, feel free to ask.

 

Craig

[chowquoe^]

+1 IntegrexMan

 

Yes, MasterCAM works excellent with the Intergrex, I have been using it now for about a year with our machines. If you need any help feel free to pic my brain as well. Just out of curiosity did you get your post from In-house?

 

[cncfrank]

Kind of, actually got it from Axsys, but I know Axsys got it from Bret at In-house. Thanks for the help....I'm sure I'll be back to pick your brains.

 

Thanks again

Frank

[Stewron]

We have many Mastercam / Integrex installations in the UK and they work well. Most have our own post developed with Mazak but some now have one from Camaix. That's a good post if you want to then go down the Camaix machine simulation route.

[CHRIS_B]

IntegrexMan, I'd like to pick your brain for a moment if you don't mind. I've been using the In-house post for a couple months on our 3 integrexes, but I'm having trouble getting an answer from them about a specific issue. When circular interpolating a hole with a live tool, I can get the post to output G41,G42,G40 in the code, but when I try to adjust the tool diameter in the tool data page, it doesn't have any effect on the hole diameter like it does in mazatrol. Am i adjusting the cutter comp in the correct place? How does cutter comp work for you?

Thanks very much

[Watcher]

If I understood correctly, you are using Cutter compensation to machine these holes. What kind of CC? Wear, Computer, Reverse Wear, etc? I think that this is the reason why when you change the tool diam. on the tool data page the code looks like the same, because depending on CC type that you choose, Mastercam creates the code based on the real dimension of the profile, as if the tool is cutting in its center, the CNC control will be responsible to compensate the moves. In these cases, the changes in the tools diameter are no effective.

 

Just my 2 cents.

 

[ 04-29-2006, 10:12 PM: Message edited by: Watcher ]

[CHRIS_B]

Watcher,

I'm using the wear comp setting in MCX. When I say change the diameter on the tool data page, I mean the tool data page on the machine. My code looks good as far as i can tell (it includes the g-codes for cutter comp) and I don't want the code to change. I want the machine to compensate for the different tool size just the way you described. Thanks for trying to help.

[Watcher]

Well, if you are using wear, I think that you have some problem.

 

Unfortunately, I cannot help.

[crazy^millman]

Ok so let me ask this question. I would think you are using the eia side of the machine to do the programs from Mastercam. If this is the case do you have your tooloffset ties to the Mazatrol side of the machine or the eia side of the machine for the tooloffsets. If you do have them ties to the eia side of the machine are you sure you are on the right page when making the adjustments. If you are making adjustments to tooloffsets on the Mazatrol side of the machine without it set-up to do so it will have no bearing on a eia program and thus no one at CNC software or In-house will be of any help in this type of s problem. A simple test do a simple pocket and then adjust the offset by like .05 your standard way you are using if nothing happens and you know the code is right then it would speak to the fact you are not using the right page. Contact you Local Mazak dealer or service center and tell them to give you the parameters to use the Mazatrol side ofthe machine for tooloffets parameters. Be very careful here and understand the full ramfications of doing this. Does this effect povits for the the multiaxis wotk and any axis substution you might be doing via eia code or Mazatrol. I think I remeber someone saying that Mazatrol will not handle wear so you must use the eia side for tooloffset, but could be wrong. Boy do I miss Mazak's.

 

HTH and I hope I am on the mark here been many years since running a Mazak, but think I might be on the problem here if not just something else to think about is all.

[Travis B]

Chris_B, Depinding on how your machine parameters are set, you might can use all mazatrol offsets. The way ours are setup I use all mazatrol offsets except for end mills. For end mills I use the fanuc type offset page and set direction to a 0 or 9. HTH.

[CHRIS_B]

That's correct, I'm using EIA programming and I did a test last week like you described. Nothing happened. My program did include code for cutter comp. I'm using the mazatrol adjustment page for all tools, endmills included and it all seems to work well except I can't get the tool diameter to affect the cutter comp and I don't see anywhere else to enter a cutter comp value on either the mazatrol or EIA side. Travis, are you refering to the "tool offset" page in the machine for your endmills? Where exactly on that page do you adjust your cutter comp? And I don't understand setting tool direction with a 0-9 value. I haven't heard of setting in that way. Is that done on the "tool offset" page as well?

Thanks alot for your help!

[Travis B]

Yes, under tool nose radius for the tool number you want to offset enter the radius offset and enter 0 or 9 for tool direction. 0 or 9 is for center of tool.

[IntegrexMan]

Chris,

 

You need to use the tool offset page for adjusting cutter comp. Not the Mazatrol tool data page. You should call up your tool as either a 4 digit or 6 digit T code. For example: Tool 1 should be T001001.00 this would be tool 1 using offset 1 in the tool offset page. This tool is in the horizotal position. 4 digit T code would be T0101.00 has the same effect. Now you would put your cutter comp offset amount in the R value for offset 1. if you want, e-mail me your code so I can look at it. Sorry the long response time, have been a little busy.

 

Craig

[CHRIS_B]

Craig,

"Now you would put your cutter comp offset amount in the R value for offset 1." Do you mean the "NOSE-R" column of the "TOOL OFFSET" page? I'll have to try that, won't have time today, though. I know what you mean about being busy!

Thanks very much for your help.

[IntegrexMan]

Chris,

 

Yes put your offset amount as a radial value in the "NOSE-R" column of the "TOOL OFFSET" page.

 

Craig

[toolall1]

you will still need an aproach vector and exit to turn on and off g41g42

[CHRIS_B]

I finally got a chance to try this cutter comp thing again and it works good. Used wear comp in MCX and had 0 in my NOSE-R column of tool offset page and it cut right to size. Then, I put -.01 in there and it took off .01 more. I tried it with C-axis contour, pocket, and helix bore. Worked just fine with all! Thanks alot for helping me find it!

[IndSolutions]

The tool radius on the Integrex can only be comped in the Tool Offset page on the machine. The X and Z wear offsets can be made effective by changing parameter P10 bit 3 to a 1.

Insert the cutter radius in the Nose Rad column on the seperate offset page. When you call a tool, you specify an offset number on the tool call. This forces the EIA Offset page offset number to be used. Parameter P10 bit 3 will add the offset called in the tool number to be added to the Tool Data page Wear offsets, but only the WearX and WearZ offsets are used on the Tool Data page.