Issues with Transform Toolpath?

[neurosis]

For some reason I have had a heck of a time with Transform toolpath today. It has crashed Mastercam about a dozen times. Not only that, but when I am able to get it to work it gives me results that would crash my machine.

 

It is sending one of the tools below Z0, which is the face of my technigrip, approx .25 for one tool only.

 

 

Before transform

 

 

After transform.

 

 

 

 

You can see the rapid move in yellow below the face of the tooling.

 

My settings are

 

Type: Translate

Method: Coordinate

Group NCI: Operation type

 

Copy Source operations

Disable posting in selected

 

-------------------------------

 

I get the same results using Rectangular or Between points.

 

I am just moving the path 5.5" in one direction.

 

Rectangular

 

X spacing 0.

Y spacing 5.5

 

X steps I have tried both 1 and 0

Y steps 2

 

 

It either crashes Mastercam or gives machine crashing results.

 

I got lucky at the machine and was able to stop the tool before it plummeted through my tooling.

 

I had already been running a single parts and was just getting ready to start running multiples.

[Matt Sumner]

What type of toolpath is it doing when it crashes? I'll try it out and see if I get the same results.

[Ray Culver]

Which version?

[neurosis]

Ray,

 

Look at my sig.. Its X4 MU3.

 

 

Matt,

 

There were three paths doing it. One is a contour, one is a drilling cycle, and one is a facemill.

[B. Rad]

Neurosis,

Do you get the same problem using the tool plane transform method. I use this one alot with a subprograms in incremental and change the G98's to G97's and the subprogram callouts from O to N. this keeps all the subs in the main program on the control. As far as tranforming drill operations I have had problems with the way the program posts, so I have to correct the drill depths in the Gcode after posting. I think it is a problem with the post I am using.

 

Brad Craig

[Matt Sumner]

Sorry for the delayed reply. I've tried a bunch of different settings and I can't repeat what you've got happening. Maybe try looking through the parameters of the problem toolpath for a 0.25" setting like a retract or something. Try changing it and see if it adjusts the problem area. If you can find a parameter that's related to the problem it might give you a clue as to what's causing it.

 

If you like you can email me the file and I'll take a look at it for you. I can't promise anything though.

[3R!< W3NG3R]

I have had this many times before, and I don't know what causes it. I have a file I could send in.

Maybe I will right now. Don;t know why I didn't before

[3R!< W3NG3R]

Logged as CNC 00077232

[Ray Culver]

quote:

---

Logged as CNC 00077232

---

Sorry for the delay - I'll take a look tomorrow.

 

FYI: Transform toolpath had a major redo for X5 (especially mirror!). You now have the option to either transform the NCI (like in X4) or temporarily transform/copy the geometry, generate and save the new NCI on the copy, and then blow away the copy (just like what you'd do if you had to do it manually). It takes a little longer, but it's always correct. This eliminates all the assumptions that are inherent when you're just copying NCI (especially when doing a mirror-reverse with all the retract and comp direction issues). The transform-mirror option always forces on the 'use geometry' option. For Translate and Rotate you have a choice.

 

Oh, and you can transform toolpaths that reference solids now too. It will extract & copy a surface from the selected solid face to machine to (it won't copy the solid - that would create quite a large mess of duplicate solids).

 

 

You ain't bonafide if you don't have a scar from a hot chip.

[cobra95kev]

Sounds awesome Ray,

Can't wait to get my hands on X5. I have pretty much gave up on transform mirror a while back, hopefully I can now start using it again.

 

A side question how about being able to mirror tool planes and WCS? Will this new transform mirror do this in the background? Or will we still need to create new planes when mirroring geo? I think it would be nice to select a bunch of Tool planes and

WCS and say mirror them about a line or system axis?

 

Thanks,

Kevin C.

[Ray Culver]

Kev,

 

It will now create (and optionally save) all the new named views transform needs to support whatever NCI (or spawned operations) are created. You have a choice to save them if not creating new operations and geometry. If you are creating new operations, this option is forced on (as we need these views to store in the operation's toolplane, etc). The system will first look for any existing matching views and use those before creating loads of duplicates though. If it does need to create one on-the-fly in transform, the default view name is XFORM_n where n is the next available number.

 

One of the problems with the old mirror option was 'mirroring a view' which created bad 'left-handed' views. Imagine a icon of XYZ axis, then think of flipping just the X axis about the Y to create a "mirror" of the original, but the Z direction must stay the same. Mathematically is doesn't work and the 1014 line in the NCI (the toolplane) would be invalid and cause a lot of users problems. We used to have to massage these bad views in backplot and verify just so they'd display properly. Basically bad news overall. The new transform fixes all this.

[cobra95kev]

Awesome thanks for the update!

[BenK]

Stop with the X5 teasers already I can’t handle it anymore. I’m very impatient person and I can’t wait until X5 is out.

[Ray Culver]

quote:

---

Logged as CNC 00077232

---

Yup, the X5 redo stomped on that bug too.

 

[Giel Kaandorp]

</font>

<font size="1" face="Verdana, Helvetica, sans-serif, Arial">quote:</font><hr /><font size="2" face="Verdana, Helvetica, sans-serif, Arial"> Logged as CNC 00077232 </font><hr />

<font size="2" face="Verdana, Helvetica, sans-serif, Arial">Sorry for the delay - I'll take a look tomorrow.

 

FYI: Transform toolpath had a major redo for X5 (especially mirror!). You now have the option to either transform the NCI (like in X4) or temporarily transform/copy the geometry, generate and save the new NCI on the copy, and then blow away the copy (just like what you'd do if you had to do it manually). It takes a little longer, but it's always correct. This eliminates all the assumptions that are inherent when you're just copying NCI (especially when doing a mirror-reverse with all the retract and comp direction issues). The transform-mirror option always forces on the 'use geometry' option. For Translate and Rotate you have a choice.

 

Oh, and you can transform toolpaths that reference solids now too. It will extract & copy a surface from the selected solid face to machine to (it won't copy the solid - that would create quite a large mess of duplicate solids).

 

 

You ain't bonafide if you don't have a scar from a hot chip.

 

Quastion,

 

I just want to mirror my 5axes program with the nci fuction, do you now wy that's not possible anymore?

 

Greetings Giel