OKUMA 5X TRUNNION G169 TCPC GIVING WEIRD NUMBER

[lowcountrycamo]

We have an Okuma mu4000 5x trunnion and post from Impostablilty.  Love the post.  We recently started using G169 TCPC so we could get away from inverse time G93.  The tool path runs as it should but approaches from the side instead of from Z.  In one case the trunnion was over at B-90. C0.    The position should have been about X8.xxx , Z2.xxx but output X2.xxx and Z8.xxx.   It did run well other than the lateral approach but this worries me, as I don't understand what is happening.  I will contact my reseller if I need to but though I might get an easy answer here first. 

Thanks very much,

Steve Austin

[crazy^millman]

Steve, really comes down to the mapping method with a process like this. What is the intent of the operation and what was the process used to get it started. Sometimes a point toolpaths or something to align the toolpath to what you want it to be and not where you expecting it to be helps. Remember Mastercam is not kinematic aware it is dumb to the machine. We are programmers have to fill in the missing pieces of the puzzle for any 5 axis operation. We may program in Top, but the operation needs to start from Front. We then might need to make a point operation for front to them do the other work. Since 5 Axis programming in Mastercam has always traditionally been from a TOP prospective it point back to my thoughts about not being Kinematic aware. It is world aware, but that is 2 different things and conversations all together, This is the work and the process we have to figure out what we need to do to make the process give us the output we need on the machine. Once we do we are off the races, but that is some times the work.

[lowcountrycamo]

So I am beginning to understand what it going on.  I did a simple 5x curve and looked at the output compared to the geometry dimensions in top plane.   The path is output as if it were cut from the top plane.  I had a 4" incremental clearance and z5." cut.   The initial z2. position comes from a "safe Z" dialogue box.  I believe this z position is where the machine first moves in x.  At work earlier today I had a z12. in the dialogue box and the machine was going to x12. first and then approaching from the right side.  

 

 

[Greg Williams]

The coordinates rotate with the part. So when the truninion is at A-90 the Y axis is the the Z axis

[lowcountrycamo]

On ‎7‎/‎21‎/‎2018 at 1:50 AM, Greg Williams said:

The coordinates rotate with the part. So when the truninion is at A-90 the Y axis is the the Z axis

I am getting better motion now accept the tool is dwelling when the B and C start and stop.  While the rotaries are moving the motion looks good but when the code transitions to and from only xyz their is a distinct pause.  Almost like it is waiting for clamp and unclamp,  but they are not in the code.  I have tried lowering and raising the tolerance and angle step and that does not help.  Greg, I have seen several of your videos I don't see this dwell in your programs.   I downloaded your files and noted that you are using feed in Unit/Min in the Control file.  No inverse.   Are you also using TCPC?   Could this dwell be coming from and In Position Check?  These are 1 year old twin machines.  I have searched the manuals but cannot find anything.  I know Fanuc much better than OSP.

Thank you,

Steve Austin

[Greg Williams]

Steve,

You need to change the parameter for auto clamp on the rotaries. The default is to use Auto Clamp not the Mcodes. I normally change these ones but please check these numbers as they are from a P200 control, I think number 3 is your problem. I have done demos with TCP, without TCP, with Inverse Feed and without Inverse feed and to be honest I don't see any real difference in the motion. Dimensions may be different, but the motion is similar.

My preference is to use TCP G169 and CALL OO88 for 3+2

1, Change to shorter path command for Rotarys M404/M403 #69 BIT 0 and BIT 1

2, Change Inverse time feed to Minutes  #54 BIT 2

3, Change default Clamp and Unclamp of Rotary's to Modal M codes not automatic

            Parameter 18 Additional axis add checks marks to boxes

4, Change Accell to Low Vibration Mode #67 BIT 5 then use system parameter G0 accell adjust

5, Change Parameter #46 Bit 0 to yes for G00 Linear Interpolation