Cutting tapers on a Sodick AQ300L? How do I set it up.

Hi Guys,

We've got a sodick AQ300L that's been a great machine for us. We cut tons of 2D stuff on it. I have never used the 3D taper functions and was never trained on it. I have a simple stamping die I want to make and I would like to cut the profile and relief with the wire. The part is a circle 1 1/2" dia with 2) .125 x .125 tabs sticking into the inside. .010 inside corner Rad is not a problem.

My question is, how do I set it up? I have the Heart NC program on the machine and we use that for our programming. I can probably get someone to post the code for me from Esprit or Solidcam if necessary.

Do you set the upper guides at a fixed distance off the part? If so, how? The machine is a 5 axis XYZUV.

If anyone has a Squircle example I could run that would be awesome.

Thanks in advance

Chris R

Hi 50BMG DUDE:
My experience is on a mid 90's A320 with the EX 21 control and manual Z so please take all this with a large grain of salt.
On my machine there was a setup screen in which you had to tell the machine where the upper wire guide is, and that was read off a vernier scale on the side of the Z axis.
The position of the lower guide was fixed and needed to be re-calibrated and manually re-input whenever the machine was serviced, including replacing the wire guides.
There was a gadget and a calculation involved.

Taper was programmed by a taper statement in the G code for constant value tapers.
You also had to tell the machine where the program plane was, so if the program was the same for the die relief as for the die opening, you'd set the height of the profile at the land height if you were cutting the die opening upside down (the most common way so you can get the slug out before the skim cuts).
The last thing you had to tell it was the thickness of the block.

If the taper was variable around the profile (which is not your case) the task could be done by writing "complex upper and lower" whereby you invoked the correct Gcode in the program (G141 and 142 as I dimly recall) and then wrote upper and lower segments linked with semi-colons.
When you simulated to see if you got the taper statement the right way round, remember on the old Sodicks anyway, that "Blue is Sky and Green is Grass); the blue trace refers to the upper shape and the green trace to the lower shape, so you could tell which was which and set the angle statement value negative or positive to get it the correct way round.

I assume that the newer machines with powered Z axis, that the machine can be calibrated and then remembers where the upper wire guide is; my new Chmer machine certainly does.
So if your machine is anything like my machine, there will be a taper screen in which you tell the machine you want to cut a taper using the taper command, input the taper value and whether it's positive or negative, input the program plane (the height at which the program is planned for) and the block thickness; the machine calibration cycle takes care of knowing where the upper guide is and remembers where the lower guide is.
Cheers

Marcus
Implant Mechanix ? Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
Clarus Microtech

Implmex

Thanks for the reply. I'll do some digging in the control tomorrow. I have a calibration block for the machine but no idea how to use it. It's about 2" square, 4" long and has a angular slot cut through the end.

Anybody know how to use the calibration block? I got thrown into the pool running this machine as the company bought it on the recommendation of a previous employee who has since left the building. The machine was sitting for a year.... I asked why we weren't using it, and was told to figure it out.

I've cut a lot of nice 2D stuff with it, it's pretty straight forward, but I know I'm not getting near all of the capabilities out of the machine.

Any help is appreciated!

Chris R

Bump to top. Still need some help with this if anybody else can chime in? Thanks!

Chris,

The calibration block is used to square the wire and set your Table to limit and Table to lower values used for taper and 4 axis cutting. The slot in the front is used with a program call linear taper data. It should be on your hard drive. This program will set your "Z" values automatically. For taper cutting, table to next is the bottom of the taper (normally 0 if your part is sitting on the table). Table to program is where you want to hold the top of the taper. 4 Axis cutting they are reversed, Table to next is the top and table to program is the bottom.

I used to program a Sodick like the one Marcus had. I ran into some difficulty programming using upper and lower contours, and he responded with a very helpful method:

http://www.practicalmachinist.com/vb/edm-machining/sodick-programming-question-wire-222063/

See reply number 8 in that thread. Again, this is for the Sodick A320D with an EX-21 control, so YMMV

t2r

I used to run one of these machines and Shane's post is accurate, the calibration program was called "LNtaperdata" from what I remember, and It has comments that describe how to run it within the program.

If you're not cutting 4-axis and just doing die relief you might not even need to run the calibration, the numbers in there already should be pretty close but of course I would suggest a test cut if you can to be sure.

I never used the Heart-NC functions, always used CAM to generate toolpaths does it spit out a g-code program?

Here's how I would activate taper cutting for a simple die relief, lets say for a block setup on the table 2" thick with 1 degree taper angle and a .250" land.


At the top of the program:

TP 1.75 (defines table to program distance 1.75" from 0)
TN 0 (defines the table to next value, in this case 0)

If you're cutting with left side compensation, at the line where G41 is activated I would add after G41

G51 (activate left side taper cutting)A1.0 (sets taper angle to 1degree)

so the line will look like: G41 G51 A1.0
if you're cutting right side compensation, it would be: G42 G52 A1.0

I think you will also need to add a G50 to cancel taper mode after the G40 (radius compensation cancel) at the end of the program.

You can also set the table to program and table to next values on the taper menu I believe.

007Rob said:

I used to run one of these machines and Shane's post is accurate, the calibration program was called "LNtaperdata" from what I remember, and It has comments that describe how to run it within the program.

If you're not cutting 4-axis and just doing die relief you might not even need to run the calibration, the numbers in there already should be pretty close but of course I would suggest a test cut if you can to be sure.

I never used the Heart-NC functions, always used CAM to generate toolpaths does it spit out a g-code program?

Here's how I would activate taper cutting for a simple die relief, lets say for a block setup on the table 2" thick with 1 degree taper angle and a .250" land.


At the top of the program:

TP 1.75 (defines table to program distance 1.75" from 0)
TN 0 (defines the table to next value, in this case 0)

If you're cutting with left side compensation, at the line where G41 is activated I would add after G41

G51 (activate left side taper cutting)A1.0 (sets taper angle to 1degree)

so the line will look like: G41 G51 A1.0
if you're cutting right side compensation, it would be: G42 G52 A1.0

I think you will also need to add a G50 to cancel taper mode after the G40 (radius compensation cancel) at the end of the program.

You can also set the table to program and table to next values on the taper menu I believe.

Click to expand...

I know this is an old thread, but I have a question about TP and TN.
Say my part is "not" flat on the table, but say ".1" off the table. The taper needs to be cut 1" up from the bottom of the part.
Would the TN=.1, and TP=1.0, does TP follow the bottom of the part and TN shifts it up and down if not on table zero?
Or would TN=0 still, but I add .1 to TP so TP=1.1??

Thanks.

brokentrace2 said:

I know this is an old thread, but I have a question about TP and TN.
Say my part is "not" flat on the table, but say ".1" off the table. The taper needs to be cut 1" up from the bottom of the part.
Would the TN=.1, and TP=1.0, does TP follow the bottom of the part and TN shifts it up and down if not on table zero?
Or would TN=0 still, but I add .1 to TP so TP=1.1??

Thanks.

Click to expand...

TP is where the bottom of the form is in relation to the table, TN is where your top form would be. So if your .1 off the table TP=.1 and TN= 1.1. This is the case as long as you are not leaving a land on the part.

jz814 said:

TP is where the bottom of the form is in relation to the table, TN is where your top form would be. So if your .1 off the table TP=.1 and TN= 1.1. This is the case as long as you are not leaving a land on the part.

Click to expand...

This is with the idea the taper has the larger end at the top correct?
If I want / Need the smaller end at the top, I would flip them?
Is it safe to just always go off the table, and if the part is lifted off the table, increase TN and TP both by the amount off the table?

TP and TN are just the positions of each plane for top and bottom respectively. And always that way round, regardless of top or bottom open. This becomes clear when we do a job which has angles of top and bottom open.

If cutting a 2D form these figures are completely arbitrary.

However if cutting a 3D form where the bottom of the plane is not the same level as the table, we usually just translate the form to the table height and the top plane to the job height.

This makes it clear when we are working interferentially because you can see exactly the path of the wire on the graphics run.

For most 3D forms we use the spatial move function and connect each corresponding point in each plane, the spatial move function requires a distance between each plane and this needs to be exactly measured from the job being cut. The spatial move command automatically inputs the values for TP and TN once the drawing has been saved.

brokentrace2 said:

This is with the idea the taper has the larger end at the top correct?
If I want / Need the smaller end at the top, I would flip them?
Is it safe to just always go off the table, and if the part is lifted off the table, increase TN and TP both by the amount off the table?

Click to expand...

As long as your taper cut is the whole face of the part (no lands on top or bottom) you can flip it either way and it won't change your TP/TN values.

Yes, having the part sitting on the table is typically best, however there are times when you just can't and as long as you have a good set up and parameters set correctly it will be just fine.