Sodick programming features

L

Luke.kerbey

Guest

• Nov 2, 2021

• #1

I’ve been flicking through the manual and have found interference checking.

Using G132 the machine cuts and re shapes a cutting path where the elements are smaller then the wire offset. As shown in the images below.

Up til now, we’ve had the design our stuff with the wire offset as a limitation.

The person who trained me was trained by Sodick but he had no meaningful previous experience. He had no idea about this.

So my question is, what programming tips or advanced features have any of you used that are worth knowing and sharing? I’m hoping someone can share something I don’t know of yet that will benefit me.

Sent from my iPhone using Tapatalk

 

Shane030173

Aluminum

Joined

May 21, 2013

Location

PA

• Nov 3, 2021

• #2

Checking Interference is such a great feature. It has saved many parts from being scrapped due to our " engineering dept ". I will say be careful with this on 4 axis cuts. In your settings you can set this to 1 which will stop the machine with an error or set it 2 where the machine will automatically fix it. I set it to 1 on the graphics when drawing the program. I have set to 2 in machine settings.


When the AWT is set to 10 our ALN's will thread in the gap after a wire break. Eliminating having to return to the thread point and dry running back.

 

L

Luke.kerbey

Guest

• Nov 3, 2021

• #3

I have a SLC that can rethread at break point. I’ve found g codes to turn it on, but not off yet… so haven’t had a go.

Can I change the settings without inputting codes, and using the settings pages?

 

Shane030173

Aluminum

Joined

May 21, 2013

Location

PA

• Nov 4, 2021

• #4

yes.... settings, user 2, upper left corner is AWT REFERENCE. Set at 00 will not thread the wire. Set at 01 will return the thread point and dry run back to break point. Set at 10 it will thread at the break point. If it fails threading there after 3 tries it will go back to back to the thread point, thread and dry run back.

 

L

Luke.kerbey

Guest

• Nov 4, 2021

• #5

Ace. I’ve got the perfect job to try this on. Thanks.

 

J

JZ.

Aluminum

Joined

Sep 26, 2018

Location

pa usa

• Nov 4, 2021

• #6

Shane030173 said:

yes.... settings, user 2, upper left corner is AWT REFERENCE. Set at 00 will not thread the wire. Set at 01 will return the thread point and dry run back to break point. Set at 10 it will thread at the break point. If it fails threading there after 3 tries it will go back to back to the thread point, thread and dry run back.

Click to expand...

When you have your AWT Ref at 10, do you have a preferred ACT-AWT TYPE that helps it thread better? I've always just let it re-thread back at the thread point, but sometimes I have to just throw in an M00 so I can manual thread at the break point if I need to.

 

Shane030173

Aluminum

Joined

May 21, 2013

Location

PA

• Nov 4, 2021

• #7

We use .010" wire so I keep that at 0. In manage, parameter, machine page there is SLIT AWT BACK. This is how far the machine moves back to thread in the gap. Factory setting is .07874". Sodick suggested changing that to .085". I left ours at .07874 because we had no issues with factory settings.

We have our connect type at 02. Standard thread with straightening process.

 

J

JZ.

Aluminum

Joined

Sep 26, 2018

Location

pa usa

• Nov 4, 2021

• #8

Thanks man good to know.

 

L

Luke.kerbey

Guest

• Nov 5, 2021

• #9

Wire thread at break point worked a treat, on 1/4 Ali plates, it worked every time.

Is there a way to get the machine to throw an alarm on the graphics page when my machining path falls outside the table travel? Such as when my job is too close to the edge.

 

Shane030173

Aluminum

Joined

May 21, 2013

Location

PA

• Nov 5, 2021

• #10

yes there is... go to edit, graphics. On the bottom right of the screen is settings, open that and a window will pop up. On the left side you'll see setting, click on that. On the right 2 tabs will open, basic and detail. At the bottom of the basic tab is LIMIT CHECK, set that to 2, click apply and you're all set.