Mitsubishi 4 Axis Wire

[edmBosto]

I am asking for some help on understanding a taper and as to why I am getting junk.

 

I programmed and ran a simple test piece and the results were inadequate.

I drew a .300 dia. at origin.

In the wire contour parameters I had the chain at .814 where as the bottom will be larger.

I set the taper to .250 Degrees.

I set my passes etc...

Posted and I believe the code looks good to me.

The post shows G41 H35 G01 Xvalue Yvalue A-.25 Z.814 M90.

 

Since a 1/4 degree has about .0035 taper/S.

I would expect the machine to show The U axis moving out to about .0035 for the taper.

I only see it moving out approx. .0018 or 1/2 of what I believe I should be seeing. Plus I watched the U change back to almost .0000 when it reach the 180 degree edge of the hole. (The dia. is 2 pcs.)

When it started burning the area of 180 deg. the U went back to .0018 approx. as it then varied again when it worked it's way to the start point in the geometry. While all this happened the V moved approx from .0000 to .0007 at various times during the process.

 

The result was I had a hole with approx. .003 total taper when I should have had .007.

 

I'll have to check the machined taper on a sine plate in the morning. But it's certainly not the 1/4 taper I had hoped for.

 

Hopefully someone will have some views on this.

 

I sent this from home and this is all by memory.

For me to be more specific on certain parameters or to show anyone the code I would need to wait till the morning.

Thank you in advance.

Vern

[ToolMan184]

it appears your taper is reading only half. Try making it 1/2° and see what happens.

[edmBosto]

Toolman, I may give that a try after I indicate the taper.

[Lars Christensen]

edmBosto,

What are you Z1,Z3, Z4 and Z5 values?, it sounds to me there where the problem lies, they are the once there are going to determen how you machine are going to approch your taper. This subject has been covered before in regards to program taper on a Mits wire, you might want to do a search.

The problem is that it is very hard to get your post to output the correct Z values because depending on where your program zero is. Also when you are posting out true 4 axis contour (upper and lower geometry) your Z3 and Z4 has to be the excact value from your machine, and if your post as default will post these Z3=0.0 and Z4=0.0 your machine will reset them and your taper will get screwed up, thats way I made my post to always post Z3=VALUE, Z4=VALUE in that case the machine will give a alarm if I have not modified them. if you are using "A" Value for taper Z3 and Z4 do not need to be in your output, but you will need Z1 for your program zero and Z5 to determen in what direction the taper goes.

Maybe you can try to post some code tommorow.

HTH

Lars

[Kannon]

everytime one of the wire guys have a problem in the tapers, its always in the z heights. But thats just from what I seen in our shop.

[Kannon]

common Lars....

beat me by 3 minutes.. your typing skills are commin around.

I surely thought I would be the first to hit the z heights!

[edmBosto]

Thanks guys,

I'll fool around with it some Wed. and throw some code up here if I see I can make the time.

Good to see some replies.

Thank you

[Lars Christensen]

Naah Kannon I cheated, we have brodband here in Upstate New York you know

[HevyMetl]

I work on makino's and have a little expierence with a Mits. The guys above are correct in what they are saying. I output no z values in my program and set-up everything at the control for z heights, and never have a problem with taper. You must ensure that the bottom of the part is at table zero or compensate one of your z values accordingly.

 

Your code is only half of the solution. You have to make sure your z heights in your parameters are correct telling the machine where your upper and lower guide heights are located. These values are typically based off of your Machine Coordinate system, not your work csys. You also have to tell the machine where the program and sub-planes are located based off of table zero. These are the bottom and top of your workpeice.

 

Taper is tricky and my machine offsets based off of the top guide height from table zero. So you won't see it offset the amout of your workpeice thickness. It should offset more than that if all of your z values are set up correctly. HTH

[Guest]

edmbosto, why don't you burn it on the fanuc wire.

[Guest]

edmbosto,

 

are you burning 4 axis or taper.if you are burning 4 axis you must have 2 contours.the only time you will have a chain height is when you are doing taper.if you are doing taper ,don't break the arc.

[edmBosto]

Del,

quote:

---

why don't you burn it on the fanuc wire.

---

Machines are too busy for that now so I wanted to try the Mit.

I did break the arcs.

I'm trying a 4 axis on the mit, but it's slower than the reg taper tpath.

My .300 dia. keeps getting larger and larger with all my experimenting.

Happy new year all and thanks for the suggestions.

I'll let you know how I make out on this.

[ToolMan184]

If its 4 axis, as Del said you have to have 2 contours, start points. Contour and thread point on top, and contour, thread point on bottom. At least I think Im correct havent done any 4 axis in MC yet.

[Guest]

toolman184,

 

you won't need a thread or cutpoint in the top geometry,just the bottom.in the top you chain only the geometry.be sure and add sync to your wirepaths.in x,if you are doing circles,you also have to break the arcs at 180 deg or it wont post out the correct u and v's.personally i don't like that because you didn't have to do that in version 9. hth for future reference.

[Roger Martin from CNC Software]

quote:

---

you also have to break the arcs at 180 deg or it wont post out the correct u and v's.personally i don't like that because you didn't have to do that in version 9.

---

Sounds like a Control Definition issue.

What are your 'Arc Break' settings on the Arc page?

[dareman]

I've always just had better luck with A comands if it's just a simple taper. I only do 4 axis cuts if I have disimalar shapes on top and bottom. Here is an example of what I do. This was for a form tool but it works well on holes and die openings as well.

 

G90

H1=.0068

M122

G92 X-.35 Y-.883

G00 X-.35 Y-.883

M20

M78

M80

M82

M84

E1218

M90

G01 G41 H1 X-.25 A-1.F.1

Y-.1

A-12.

X-.183

A-6.

X-.168 Y-.115

A-12.

X-.088

A-6.

X-.083 Y-.11

A-12.

X-.068

A-1.

Y-.2723

A-12.

X.25 Y-.5903

A-1.

Y-.883

G40 M91 X.35

M91

M85

M83

M81

M21

M02

[Guest]

roger, it is set to break arcs at 180 deg.it still won't post out the correct u and v unless i manually break the arcs.is something set wrong?it is not breaking the arcs.

[edmBosto]

These are my settings.

Roger do you think I should chage something here?

[edmBosto]

Update, It's not solved yet. But I'm still working on it.

 

[ 01-03-2007, 01:26 PM: Message edited by: edmBosto ]

[Lars Christensen]

How are you making edmBosto?

[edmBosto]

Hey Lars,

I had to take a break from it as I still don't have it. I need to do some reading in the Mit book. What I,ve noticed is the Z settings don't

seem right in the machine.

My buddy says if he needs an accurate taper he runs it in the Fanuc wire. I just want to do this the right way.

I'm going to have to set those Z1, Z2 etc. and try this out.

I just got 2 of my post working pretty good with the expertise from our reseller and I want to prove some settings working on various toolpaths.

Since the posts were changed I've been dealing with non symetrical geometry for shutoff dimensions on molds that should be symetrical but I can't change the geo. to my liking since in yrs. down the road they need to replace the parts they'll have a problem.

This type of problem comes from the product designer. Then the mold designer takes it from there, then it's our turn to deal with it. It makes the job take longer to build.

[Lars Christensen]

Yeah the Z heights are critical on the Mits, however when you got them set I would predict you will have just as good luck on the Mits as you would on the Fanuc wire, we are running Mitsubishi FA's here and I see just a good results as I have had in the past with Fanuc, Charmilles and Agie's.

 

Good Luck

Lars

[Roger Martin from CNC Software]

"Z heights are critical on the Mits"

 

+1000 to that!

 

Your G-code can be perfect, but if the Z hgts are setup correctly, you are not going to produce the desired taper on that part.

 

You have to do the same on 'other' machines,

it's just they use different methods to accomplish the same function. (e.g. 'W', "H', "R" on a Charmilles)

[edmBosto]

That all makes sense since the taper is incorrect.

Thanks guys!

[Guest]

edmbosto, do you have the u and v at zero on your machine at the start when you run that program?