Sandvik Coromant Twin Tools and an Okuma Multus

[Mick]

Is anyone out there running Sandvik Coromant Twin Tool turning tools on an Okuma Multus? And running Vericut?

 

I'm keen to know how you have this working.

[Watcher]

Vericut does not have an off-the-shelf solution for this yet... I've asked them to add the ability directly in the tool manager driven point feature...

 

http://www.cgtech.co....php?f=2&t=1829

 

http://support.cgtec...28&p=4574#p4574

 

A workaround is to customize the tool change sub-routine...

 

This is how I made it work in Vericut - (For our Integrex e1060V) - I added the following code to the tool change sub-routine that comes with the Mazak template control...

 

In Mazatrol, we use the following format to tool change and offsets-> Txxx.yyy - Where xxx is the physical location in the chain magazine and yy the lenght/dimensions offset #...

 

Mazak allows you to use more than a hundred offset numbers, and if you have a big chain magazine, more than a hundred tools as well... so we wrote this:

 

...

 

( ********************************************************************

(VERICUT CONTROL MCD SUBROUTINE: Tool Change)

(Called by M06)

 

CGTECH_MACRO "SubroutineSequence" "Toolchange"

 

IF [#4120 EQ #51999] GOTO 999 (If New Tool is same as Current Tool, no tool change)

 

(Driven point in Mazak is by default the T number - So T01 = D1 / T05 = D5, and so on...)

CGTECH_VAR INT SaveCurDrivenPointNumber = #4120

 

.... -> A bunch of code not related to this issue in between

 

.... -> And below the last lines of my sub-routine

 

 

#51999 = #4120 (Save current tool)

 

N999

#8888200 = #8888100

IF [#8888200 NE 2] GOTO 999999 (Check if is a Turn Tool)

#99992000 = #99992000 * 1000

GOTO#99992000 (Value of variavel Txxx.yyy)

CGTECH_MACRO MessageMacro "Tool without a FLASHED tip - Spindle angle defined as 0 degree - Risk of collision !!!" 1

N999999 A0 M99

 

(Here is number of Tools and orientation on A axis - Format xxx.yyy)

N001010 A0 M99

N001020 A180 M99

N002010 A0 M99

N002020 A180 M99

N004010 A0 M99

N004020 A180 M99

N005010 A0 M99

N028010 A0 M99

N030010 A0 M99

 

(End)

 

8888xxx is a variable where we store the tool type - You can get that from the tool manager - You'll have to add this to your Okuma control file - Read the macro help - Macro "SetDynamicVars" option "CurToolType" - We are storing the result in the variable 8888100 as we need to check this only for turning tools in the sub-routine. - #8888200 is just for comparison purposes...

 

If you have flashed, multi-tip tools and twin tools, you have to enter a record for it in this sub-routine... xxx for pocket number yyy for offset number and A for the spindle angle of that given offset number...

 

So if you have this:

 

T1.1 M6 (Spindle at 0 degrees)

T1.2 M6 (Spindle at 120 degrees)

T1.3 M6 (Spindle at 240 degrees)

T45.121 M6 (Spindle at 45 degrees)

T45.125 M6 (Spindle at 225 degrees)

T125.45 M6 (Spindle at 60 degrees)

T125.47 M6 (Spindle at 180 degrees)

T125.50 M6 (Spindle at 300 degrees)

 

Then the table above would be:

 

(Here is number of Tools and orientation on A axis - Format xxx.yyy)

N001010 A0 M99 (T1.1)

N001020 A180 M99 (T1.2)

N001030 A240 M99 (T1.3)

N045121 A45 M99 (T45.121)

N045125 A225 M99 (T45.125)

N125045 A60 M99 (T125.45)

N125047 A180 M99 (T125.47)

N125050 A300 M99 (T125.50)

(End)

 

It's a very elegant workaround IMHO and works like a charm... you can adapt the idea to what the OSP requires...

 

HTH

[Mick]

Thanks for the comprehensive reply Daniel.

[Jeremy Herron@DBS Solutions™]

Sweet Daniel! I might plagerize you that.

[Watcher]

Glad you liked it...

 

The good thing with this workaround is that your tool manager does not need to be fooled and your CTL file remains intact...

 

The con is that every new tool in your magazine will require a record in this sub-routine, wheather you have a flashed tip or not... otherwise this line CGTECH_MACRO MessageMacro "Tool without a FLASHED tip - Spindle angle defined as 0 degree - Risk of collision !!!" 1 will be executed...

 

I hope CGTech will put this as an out-of-the-box feature in the upcoming releases...

 

Cheers,

[Mick]

Ok, the issue I have with the Twin Tools/Vericut/Okuma is as follows:

 

The Tool Angle works fine, the Tool Orientation (Okuma uses M602/M603 to index the tool), but I am having trouble using two driven points, one for each insert. The first driven point works fine, but only if I include the Y-20 coordinate in the driven point to achieve centre height, and provide a Y0 in the programme. If I don't, and put the driven point at Y0 on the tool in the tool manager, and programme the Y-20 (which is how it is done), I get an error of "insert of tool loaded is off turning plane while attempting to cut stock"

 

And when the tool indexes to the other insert, it still tries to turn with first insert (moves up on Y).

 

Does that make sense?

[Mick]

I've got it to work indexing properly and using what looks to be the correct driven points (how can I check that what driven point is being used at any given time?)

 

The only issue I have is Vericut is still reporting the "off turning plane" error

[Watcher]

What version are you using?

[Mick]

Vericut? 7.2

 

I've got rid of the turning plane error. I remodelled the insert so it didn't have negative rake. I've also got the indexing and centre height issue working good.

 

The only problem I have now, is the the tool isn't turning to size correctly. It is programmed to turn to diameter 63mm, but the Vericut reported size in XCaliper is 63.2477.

 

If I change either driven point, or the gauge length, it doesn't change the size though. I'm not confident that it is using the driven point correctly. This wasn't really covered in my training (isn't that always the way .... )

[Watcher]

I was going to ask you to check the negative angle... the only way to work with modeled inserts is importing the tools using the STEP interface... then Vericut extracts the outline of the insert and projects it onto the XZ plane...

 

Are you using a parametric insert or a modeled one? (3D, STL, etc...) - Diameters will be cut wrongly if you are not using a parametric insert... that's because the imported models are tesselated... CGTech is working to improve this...

 

The other thing are the proper macros to update the driven point when B changes... regardless the lengths, you need to update them when B changes...

 

Another feature that can help is "Qualified dimensions" - It was added in V7.2 to help with these issues...

[Mick]

Hmm, I imported the tools using the STEP interface. The insert was part of the STEP file. I ended up recreated the insert parametrically.

 

You are correct, as the diameters appear to be cut incorrectly.I've tried tweaking the drive points.

[Watcher]

In the last VUE I was told that "Qualified dimensions" can be used to workaround the problem with non-parametric inserts... however they said it's being honned yet...

 

It's weird that you got "off turning plane" error using the STEP interface... are you sure you selected the 3D insert as "Insert" and selected the cutting face before hiting "Apply" ?

 

Anyway, we decided to go with parametric inserts for everything because Vericut is still imature for 3D inserts... parametric ones are around for many years and they are proven technology...

[Mick]

Yes, I definitely defined the 3D insert as "insert" and I selected the cutting face, and then hit apply.I might looked at the Qualified Dimension option, and try that.

 

It sure is a learning curve . I appreciate your help with this