Wire Enable Finish

[edmBosto]

Just wondering if anyone else has this situation in wire.

I'm doing a no core wire toolpath with the "Enable Finish" selected and I have it doing 3 skims. All looks great in backplot.

I post it and the NC looks good as far as I can tell but the Fanuc wire machine will not except the program.

So I changed the "Enable Finish" to "Add Finish Contour" send it to the Fanuc and all is well.

The part comes out perfect. This happens 100% of the time for me.

 

I have the "Finish Pass Spacing" set to zero since the wire machine will take care of the spacing with its power levels.

Just wondering if I'm missing something here,

or if anyone else has this happening and it's a bug.

Thanks in advance for any replies!

[Guest]

edmbosto,

i never use enable finish.i always use add finish contour and reset my starting pass number to 2,if i want to skip the rough pass in the finish passes.

[Guest]

edmbosto,

to follow up, the way i see it,if you use the enable finish,you have to tell it how much stock to leave for each pass since you will have no offsets.as far as i'm concerned cnc could have left this feature out.

[edmBosto]

Del,

I actually expected you to reply!

Thanks for your valued input as that's also what works for me but the Enable Finish seems as it would be faster to program when there a # of no core burns. I just can't get it to work that way so I do it the way you also mentioned.

[edmBosto]

Del,

Soon I will try it with some sort of value in there just to see if the machine will accept the program. Maybe I'll try a .0001 Finish Pass Spacing for starters.

[Guest]

edmbosto,

 

what alarm does the machine give you.also if you have multiple nocore wirepaths you can window all of those and have only 2 operations.

[edmBosto]

Del,

Ok I'm really on to something here LOL.

________________________________________________

Quote:

(if you have multiple nocore wirepaths you can window all of those and have only 2 operation)

________________________________________________

 

Cool, Yes I agree and do understand that. But...

When I do do it that way I can only get it to work to cut and thread the wire twice as many times as I desire. Maybe you know of a way to get around that?

 

 

The notice I get is "Correct draw cannot be done"

when choosing enable finish.

[edmBosto]

Del,

I'm thinking that your Fanucs thread really good,

and it's no big deal to have the paths rough each contour then go back and finish each contour.

[Guest]

edmbosto,

 

my wires do thread very well.

i figured out how you can use the enable finish so

you can no core and finish your holes before moving to the next one.

 

lets say you have 5 holes that are .060 dia and they are one inch apart.

your material is one inch thick and you want to take 3 skims.

 

look at the ai set screen and see what your first offset is for that condition.

on mine it is.00814.

take that number and multiply it by 2 and then add

.002 to that.the .002 is for overburn.

.00814*2=.01628+.002=.01828

wirepaths>nocore|>window||>enter search point

uncheck associate to library and enter .01828 as your wire dia.for the first pass only.

 

next screen make sure that auto entry and auto exit are checked

 

lead in/out

set line length to .030

auto pos cut pt. and start pos auto set to thread pos. checked

 

roughing finishing

true spiral

check enable finish

finish pass spacing set to 0.0

check optimize

wire comp set to control.

 

this will core out the hole and then take 3 skims.

part of program

O1500

G0 G90

M31

G77 P1

G92 X0. Y0.

M60

M37

S1 D1

G1 X.00114

G3 X-.00571 I-.00343

X.01029 I.008

X-.01486 I-.01257

X.01943 I.01714

X.00675 Y.01973 I-.02171

X.02086 Y0. I-.00675 J-.01973

X.00675 Y.01973 I-.02086

G1 X0. Y0.

M37

S2 D2

G41 X.03

G3 X-.03 I-.03

X.03 I.03

G40 G1 X0.

G1

M37

S3 D3

G41 X.03

G3 X-.03 I-.03

X.03 I.03

G40 G1 X0.

M37

S4 D4

G41 X.03

G3 X-.03 I-.03

X.03 I.03

G40 G1 X0.

M50

G0 X1. Y0.

G92

M60

M37

S1 D1

G1 X1.00114

G3 X.99429 I-.00343

X1.01029 I.008

X.98515 I-.01257

X1.01942 I.01714

X1.00675 Y.01973 I-.0217

X1.02086 Y0. I-.00675 J-.01973

X1.00675 Y.01973 I-.02086

G1 X1. Y0.

M37

S2 D2

G41 X1.03

G3 X.97 I-.03

X1.03 I.03

G40 G1 X1.

M37

S3 D3

G41 X1.03

G3 X.97 I-.03

X1.03 I.03

G40 G1 X1.

M37

S4 D4

G41 X1.03

G3 X.97 I-.03

X1.03 I.03

G40 G1 X1.

M50

G0 X2. Y0.

G92

[edmBosto]

Del,

Thank you for checking this out. I can look at this tomorrow. Do you like the idea of roughing and finishing the holes then moving on to the next hole location?

When I had seen your reply my reation was WOW!

[HevyMetl]

I only do this if my parts will be out of the tank within the day. I don't like finished parts setting in the tank when other parts are cutting. I have expierenced pitting in the past when the machine has ran over night with finished parts. I usually rough everything and then come back and skim the parts.

 

My wire blocks are 3" by 6" by 1" tall and I usuall get between 50-150 parts out of 1 piece.

[Guest]

i agree,i would prefer to do all of my finishing

at last if parts are in the tank for a long time.

i don't have any problems with d-2 or a-2.4140and p20 is bad about pitting.

[HevyMetl]

P-20 is a big time problem. I would prefere to make everyting out of prehard H13 if P20 is called out. There are some really good grades out there and they have better properties than P-20. If I have to use P20 I get it from International Mold Steel and it is called PX5. It is good stuff.

[edmBosto]

We just save our cutting off for the morning as the mold and die steels we use don't pit where it's a problem for us. But I see from your responses some steels do pit too much.

[edmBosto]

Del, .

I tried what you showed me;

Quote:

_________________________________________________

i figured out how you can use the enable finish so

you can no core and finish your holes before moving to the next one.

_________________________________________________

 

Of coarse it worked and the machine drew it fine.

You knew it would if I followed your directions.

Thank you.

 

This is what I do;

I have my no core power setting (1st pass only)

set to .0100 wire dia and .007 stock on stock to leave. I finally got the machine to draw it this way also but only because I had to uncheck "associate to library".

 

That's why it didn't take the program.

Those little check mark boxes can get you working harder than you need to at times.LOL

 

The important thing is I learned from this. Your way of telling the wire size is larger reminds me of the times I told v9 mill 3 toolpaths that the cutter was smaller than it actually was.

By the way that machine I use to run "the Bostomatic" was sent to Texas at the beginning of this year and now I'm in wire for the time being anyways.

 

I'd certainly like to hear some more wire chat in the near future.

Thanks all for responding.

Vern

rock on!

[Guest]

edmbosto,

 

i could not get it to post correctly using the enable finish by telling it in the associate to library how much stock to leave.it would then leave that much stock on all of the finish passes also.that is why i increased the wire dia. in the first pass only.if you tell it to leave .007 stock

and you are burning a .060 dia hole you will see that the wire only moves to x or y .023 while using offsets on the finish passes.be careful. i think it is best to use the add finish operation.you do however tell it how much stock to leave for the no core passes in the associate to library.i usually make this .002 and reset my pass number for the first skim pass to 2 in the wire power library.hope this makes sense.

[edmBosto]

I was believing that was a graphics issue as to it showing it leaving stock on the finish passes in backplot. Yes the prog. would show the shift. Duh!

 

What you stated in the last message does make sense.

I'm going to see how this works since we use

S0 D0 (Esprit)on our 1st roughing pass then S1, S2, S3 for the remaining. I don't use Esprit but my buddy does. I use only mastercam.

 

I now have the wire dia. set at .024 for the 1st pass not associated with library.

and then having the wire dia. .010 for the remaining passes and letting the machine offsets do the work. The offsets on the nc file looks good but I don't see the S1 D1 again since it is already in effect. If you know what I'm saying.

This is with enable finish checked.

I want to give this a try as it should be good.

[Guest]

edmbosto,

i use s0 d0 only if i am taking one pass only.

those power settings and offsets on the fanuc wire are set up that way.

[edmBosto]

We use S0 D0 for 1 pass also.