[kopsik]

Hello

I'm having some problems using our 4th axis (HRT160) on our Haas VF-2.

First of all when I need to mill a tube on all four sides and I make my toolpaths using tool planes I get an error - the tool can not be positioned within machine rotary limits. ( I am using generic haas vf-tr series 5 axis trunnion mill)

Second problem is that I need advice on which toolpath to use when I need to mill a round bar using the 4th axis as seen on the attached picture.



Thanks in advance.

[Superman]

OK, first things first

Is your machine a 5-axis or a 4 ?
What are the rotary axis addresses, & what linear axis do they rotate around ?


Typically, the WCS is the setup of the part on the machine when all rotary axes are at ZERO, & this WCS is used on all operation for that setup.
Any T/C planes must be legit views capable by the machine when using that WCS. For example, if one view is rotated 180° around Z, the machine is not capable of achieving those angles & would give an error

Until the setup issues are correct, it is then possible to then to see if the actual machine (MMD) file has been done correctly
the 90° maximum could be a result of incorect WCS & planes usage

[kopsik]

The machine is 3-axis plus rotary indexer which rotates around the x-axis. It is positioned on the left side of the table (It seems that in mastercam the indexer is ment to be by default on the right side and all my rotations are the wrong way around).

[Superman]

So, you have a rotary axis along X, Do you call it A ?

But.....why do you have it under the toolchanger ?????

- when the machine homes to the rear left corner, you have access to the whole table.
- if the tool is too long, you've crunched the tool & A-axis, or you are really restricting your machining capacity
- if clamp/unclamping, you are getting too close to sharp edges
- it is the end where the swarf is evacuated

I'd say standard placement is the head on the RH of the table, like the attached image


plus...why a 5-axis post ?...you may be better to use a 4-axis post so that you don't get code for a 5-axis machine

[kopsik]

The indexer is placed on the left side because on the top right side is our OTS probe.

We use the 5-axis post because the code looks nicer and it doesn't have a X0. command during tool change and at the end.

And yes I call it A-axis.

PS! I am a complete newbie when it comes to milling+mastercam. We have had the machine for almost a year now and we learn as we go.

Our Haas mill

[Delw]

Haas makes a riser for tool setter when using a 4th axis,
its made out of 3/4" or 1" alum and extreamly simple, you can make one in 1 hour no problem and be just as good. I have one that came with my machine but never used it.

2 ways to make your part , its a very simple part. make it in 2 operations(index 180 degress) or in 4 operations (index in 90degrees)
aside from that the easiest way to make your part round and do te work you need is with a 3axis,post you dont need a 4 or axis post.
surface the radius parts, (using a ball endmill) and blend them to each other) the flats get done normally with a flat endmill.
thi is a very simple part.
if your Tol is tight on the rad. then do it in 4 parts ie 90º increments. you dont need the 4 axis to turn except for positioning only.
sometimes we tend to make 4th axis work to complicated whihc leads to major problems and time consumption. with a 3 axis post you just add in the index degrees manually.

Delw

[kopsik]

I ended up using the wireframe swept 3d toolpath with a 12mm 0.2mm radius endmill and a stepover of 0,1 mm. Got the surface nice and smooth.

Now the only problem is the rotary indexer and getting the programs to work beyond 90 degree rotation.

I called our Haas rep and he's going to stop by and reposition the OTS probe so that I can put the indexer on the right side of the table and do some other minor tinkering and repairs - noisy coolant pump, some leaks.

[Superman]

The reason you are not getting anything past 90° is ..you are using a 5-axis post meant for a trunion machine
the trunion ( A-axis---usually has a limits of +20° to -110°) & a C-axis ( full 360° rotation )

---this is why you should be selecting a 4-axis machine MMD file & post

Your process operations & views may be correct, but the post & the MMD file are wrong, so you would have to do major changes to get correct code.

For starters, open the MMD file & follow the highlighted areas. This should reverse your A-axis

[kopsik]

Now my indexer is placed on the right side of the table as per Supermans attached picture. Tried to use generic 4-axis mill but now I am getting an error - X over travel range when I load the program into the mill - part zero is in the middle of the table and tool travel is about 150mm/6inches and there is no reason for that kind of an error.

[Delw]

check your work offset to make sure you are using the same one in your machine( the one you set) and program. usually its the g54-g59, I think the defualt on mastercam is g54

[kopsik]

I checked the NC code and just as Delw said, the work offset for the firs op was G54 and the second one was a G53 which was the problem.

I tried a quick part with three toolpaths and three rotations. Every new toolplane had a new work offset - G54,G55,G56.

So I changed all the offsets to 0=G54, but now mastercam gives me an error regarding multiple 0 offsets. I ignored it and ran the graphic simulation on the mill. The program had 3 toolpaths with 0, 90 and 225 degree rotations. The 0-degree toolpath was in one place and the 90 and 225 degree toolpaths were about 10inches to the right. On the part they were on top of each other.

[Delw]

post your code
as there is no 0=G54 in any machine code.

the machine code should just read g54 or "g" what ever.
I am assuming you know who to read "G" code. if not find someone who does or learn it fast, before you touch mastercam again. your going to damage your machine beyond repair if you dont know what your looking at on the code.

HAAS has a fantastic book on g code. look in the haas section, use it for reference.
one of the best ways to learn G code fast is to print out the code on paper and go line by line what each code does comparing it in the book use a high lighter and make notes on that printed paper.
I will try to find the manual link

[Delw]

http://www.cnczone.com/forums/haas_m...irst_haas.html
towards the botton theres a pdf file.

Print it out, preferrable take it to an office supply place have them print it and bind it.
best reference tool around for people who dont understand or new to g code

[kopsik]

No need to panic. English isn't my native language and sometimes I express myself a little bit unclearly.

By 0=G54 I meant that in mastercam, under planes, I changed the offset to 0 which in the post file means/is G54.

[Delw]

according to mine 0-1= g92 and 2= g94's under planes

Delw

[kopsik]

The attached picture shows where I changed the offsets.
040.txt is mastercams original code using three toolplanes(G54,G55,G56).
040_0.txt is the same, but with the offsets changed to 0 (everything is G54).
When I change the offsets to 0, I get an error - see attached error.jpg.

I know that I am doing something wrong.

[Rstewart]

post your code
as there is no 0=G54 in any machine code.

the machine code should just read g54 or "g" what ever.
I am assuming you know who to read "G" code. if not find someone who does or learn it fast, before you touch mastercam again. your going to damage your machine beyond repair if you dont know what your looking at on the code.

HAAS has a fantastic book on g code. look in the haas section, use it for reference.
one of the best ways to learn G code fast is to print out the code on paper and go line by line what each code does comparing it in the book use a high lighter and make notes on that printed paper.
I will try to find the manual link

No, He is talking about the settings in MasterCam. 0= G54

If you use the Free Mpmaster Post that you can get over at eMastercam dot com. You can tell the program to Lock on to First Work Offset which I always do for 4th axis stuff.

You definately DO NOT need to be using a 5 AX post!! Thats crazy

It is very easy to comment Out the G28 X0. thats in the post.