ref points driving me crazy

[jlw™]

is any one else having trouble with ref points not displaying and posting correctly?

For example, ref points that are unchecked display on the screen or ref points that are checked do not display on the screen.

Same with posting, which can be VERY VERY BAD.  This has almost burnt me twice.  Fortunately the guys at the panel were watching.

Save, regenerate, repost usually fixes it but sometimes it takes multiple attempts of that.

This has interrupted my workflow more than anything else in all of mastercam the mastercam bugs I've found.  I use ref points on practically every op one machine.

[Machineguy]

is this in 2018?

I use ref points for the lathe so I don't hit the tail stock. Rapids will go right into it. I use them as rapid points.

I turned the safety area for the tailstock way down so I can get the longer tools in the turret of the SL-10 Hass.

z in this machine is only 12" max. Makes for some interesting programing at times.

[jlw™]

I have not seen it in lathe, only milling.  I have seen it since X8 (I started using mcam w/ X8) but I understand it goes farther than that.

[gcode]

I see this frequently.. and it can be very dangerous ... a failure to post Reference points can lead to catastrophic crashes

Sometimes they just won't backplot or post with no rhyme nor reason why

There are three solutions that I know of

1 don't use them

2. rebuild the op from scratch

3. Close the file,

   go to System Config/Files page

  Uncheck "Restore entire toolpath data in File, Open"

  reopen your file

When you do this, the entire file opens dirty and must be regened,

This normally works, but can be impractical and time consuming if your file is three or four hundred

surfacing ops with lots of stock models

 

I'd love to be able to replicate this issue so QC could kill it for good

Its been around since the introduction of Reference Points

It's much better that it used to be, but still requires extreme caution when using Reference Points

   

 

 

[jlw™]

Usually save, close, reopen and regen affected ops works for me.  Sometimes it takes a few times.  This could have burnt me several times if the guys at the panel hadn't been watching.

This single bug costs me more time than every other issue combined.  I'd say 20% of every job I program is dedicated to correcting this.

[MIL-TFP-41]

I gave up using them a while back. I use a point toolpath instead....& even those can be picky sometimes.

[jlw™]

I really have no choice.  I have a head/head 6 axis and have to position XY after rotary before W and I use ref points in  my post to position with G68.2 and tool length.  I have to sneak all over a 236 in table all the time.  I often split travel limits by 0.05in and have to position with tool lenth to prevent overtravel or worse

[Tim Johnson]

How do you guys use reference points? I use them all the time but I create point geometry and click on the point I'm referencing to. If I move the point for whatever reason the reference box will show the new position.

[Guest]

I have a 2017 file with 55 reference points....

I enter a value as I am only using it as a Z retract......gone through the code, all are present and accounted for.....

On this I just entered a value.....but curious how others are seeing the issue.

[jlw™]

Sometimes I key mine in, sometimes I create points and click.

[JohnW@Kauffman]

47 minutes ago, Tim Johnson said:

How do you guys use reference points? I use them all the time but I create point geometry and click on the point I'm referencing to. If I move the point for whatever reason the reference box will show the new position.

I use reference points primarily for Z control on retract and approach moves.  If I need to control A and C axes also, I create a small circle, rotate it to the desired angle, create a plane using the rotated circle, then create a point toolpath using that new plane.

[Newbeeee™]

I'm still using X9 and it's been rock solid.

We use them for rotary work (4th axis VMC) to retract in Z only, or for the smaller machines retract in both Z and X so the toolchange doesn't tw4t the part.

This is always text entered into the box and it's never failed. We have never used clicky pointies though.

[jlw™]

For the record, I had the problem from X8 up.

[#Rekd™]

1 minute ago, jlw™ said:

For the record, I have a problem

Fissed for accuracy!! LMAO!

[jlw™]

Thanks for fisting that for me.

[Guest]

38 minutes ago, jlw™ said:

Thanks for fisting that for me.

Really got to know Bubbles on a different level I see

 

LMAO

[huskermcdoogle]

I knocked a spindle out of a machine with this bug back in X4 days....  Still gives me trouble to this day.  I need to spend some time and see about  putting a warning in the post to check it they were output or not.   I look at all my posted code null tool changes every time I post code to the machine.  But mostly I avoid ref points now unless I am going from one side of the part to the other now, and I never let the machine fly through those sections of the program.

[Newbeeee™]

2 hours ago, jlw™ said:

For the record, I had the problem from X8 up.

didn't you start mastercamming @ x8?

[jlw™]

LMAO, yes yadick.

[Guest]

[huskermcdoogle]

So, I have done some digging on prmcodes for ref points.  I have figured out the codes for when the main checkboxes are on the settings for which direction and abs/inc, however I havent found much reference to the numerical values that are entered into the box 10080<>10082 and 12259<>12261.  Are these in world coordinate, or in your tool plane in relation to your OP WCS?   So I will have to do some thinking on how to implement a post warning based on those settings, with the lack of some easy targets to compare against some help on some logic to follow would be greatly appreciated.  I would like to create a post block for those of us that struggle with this issue so we can copy and paste into a few places in our posts to accomplish this check.  I couldn't find anything from previous posts where this was solved in the post.  

Last time this issue made it to the machine for me it cost $40k.

[Newbeeee™]

Husker - would I be correct in saying the values are related to your Tplane. If you do a simple check - toolpath something in TOP and put a Z value as a ref.

Copy that operation to say BOTTOM and change your plane, and then look at the value that is in your retract.

It will have changed.

 

[huskermcdoogle]

Some quick testing has yielded a pretty strong theory that the values in the opcode output are in world top, regarless of plane settings or origins.  So that being said, shouldn't be terribly difficult to do some maths using plane information to compare values against output values.  Output values in the nci are in the toolplane reference.

[huskermcdoogle]

This issue of these ref points not regenning into the nci therefore not has to be one of the most annoying, dangerous, and time consuming long lasting issues ever....   Ugh, I just had to do the gcode method 3, then by mistake hit the regen dirty ops button.   I have some unsaved work for a fix I just made...  I think it will be best to kill this puppy, and do it over...  I need to delete the unneeded stock models out of this thing and save/import an stl so this stops being a problem.

Anyone care to help me do generate the math on the points so I can develop a post patch for this problem?  I'm willing to blast out the majority of the code, just need help making it work.

[crazy^millman]

Just had my fight with this today putting the final touches on a part in 2017 that was a 4 month project. I just old schooled it and created point toolpaths. Nice when engineers think .4 and 1.2 degrees angles for holes on a Datum are needed. I was gouging and could not figure out for the life of me why. Then zoomed in on one of the 40 cross sections to see the angle difference on the holes on a compound angle surface the holes and then at angels to them.