transform operations

[AMCNitro]

Can you transform a transform?  In other words, can I rotate a Finish Scallop and then mirror it?

[Sticky]

Yep, but be forwarned, it doesn't always work as it should, it can be buggy.

[AMCNitro]

Ive been doing a lot of transform lately and in some instances it will do it but it will create extra geometry, circles lol

[Fred @ Slate Industries]

You could

Do exactly that to the geo on another level.

Copy and paste the original toolpath and then re pick the geo to the mirrored etc.

 

Or....?

[jlw™]

Maybe I flex my clicker muscle too much but I'd rather clickity click than whamity wham a machine on a lazy factor.  I don't even like transform but I will do it in the right application.  I prefer to copy a path and rechain.

[crazy^millman]

I have had as many as 4 deep in transforms with no issues. A transform for a pattern, then one for a rotation, to machine as many as 100 parts with 3 or 4 parent operations and then 3 transform operations. I just did a RAH transform rotated where I had it increment 5.5 degree for one operation 5 times. Then transform rotated -5.5 degree for another operation 5 times. I then transformed rotated those operations 7 times at 45 degree. I ended up with 80 machining operation using 2 seed ops and 3 transform ops. Same part had many operation transform rotated 7 times.

[crazy^millman]

Double post

[Colin Gilchrist]

I think Transform Operations are one of the most overlooked and least understood functions in Mastercam. I've been doing a ton of Subroutine Post Processors lately for various shops, and most of these good Programmers have never used Transform before. So in addition to modifying the Post Processor to output the formatting they want, I end up doing training sessions to teach them how to setup and use the Transform Operations to get the Subroutine output they want.

 

I always get "well why would I use a Transform to do that? Couldn't you just modify the post and let me output regular Operations?" Sure, but the Transform Ops make it much easier to scale the output. If you want 3 stations, each running a different Work Offset, on each side of a Tombstone, then Transform makes it easy to setup and to modify. Oh, you added an extra vise to the setup? No problem, just go into the Transform, change the number of instances, Regenerate and Post. It makes it easy to control the "Main" calling program, and the Subroutine output options as well.

 

One of the only things that has been a limitation in the Transform Op is the "symmetrical" nature of the patterns. There is really no way to go "point to point", where there is a unique distance between each feature. You can do a "rectangular" pattern, and you have some "sorting" options about how the tools move from station to station, but you can't just pick random points and repeat the feature at each custom location.

 

I got around this by modifying a Custom Drill Cycle to output the "Pattern Calls", where each drill position is essentially a "G65 Macro" call, and it passes an XYZ location to the Subroutine. So I can have a Main Program that repeats the main call with a different Work Offset number, but then the individual Subroutine that gets called can call the "Pattern" Sub. This can be of an arbitrary length, since it is tied to the Custom Drill Cycle, and each Pattern Position just passes a new XYZ location to another Subroutine that cuts the feature. It gets a little complex to setup and keep track of multiple nested Sub calls, but the end result is amazing for the Programmers that want that capability. Basically, call up a Work Offset, and then repeat a Sub Program that cuts a feature at any number of chosen locations that do not have to be Symmetrical. Oh, and if you need to "skip a station" for some reason, just use the Toolpath Editor to place a Block Delete (1-9) in front of that Pattern Call. Some of the programs will put multiple different block deletes in front of the lines. For the first Work Offset in the Main Program, no Block Delete. Then /1 in front of all other stations, so you can just run only the first station on each side of the tombstone. But in the nested Pattern Repeat Sub, add a "/2", or "/2/3" in front of the line. You can really get creative if your machine has multiple block delete commands, and especially if it allows multiple block delete switches on the same line. It is also really nice to be able to just output the entire program, based on the settings inside the Mastercam operations, without having to hand-edit a single line of code...

 

A quick sample might look like this:

M0 (WARNING - CHECK BLOCK DELETE SWITCHES!)
#3006 = 104 (ASK SUPERVISOR IF UNSURE)
(FOR -1, -2, -5, -7 - TURN OFF ALL EXCEPT /1 OR /2 - STATION SKIP ONLY)
(FOR -223 P/N, SET /3)
(FOR -55 P/N, SET /4)
(FOR -554 P/N, SET /3 AND /4)
(FOR -77 P/N, SET /4 AND /5)
(FOR -3 P/N ONLY, SET /3 AND /4 AND /5)
#3006 = 105 (WARNING CHECK SWITCHES)
#3006 = 106 (YOU COULD BE WRITTEN UP!)

(FEED ADJUST FACTOR)
#535=0.95

N103 IF [#4120 EQ 3] GOTO 333
T3 M6
N333
G0 G90 G54 X0. Y0. B0. S2200 M3
G43 H3 Z3. M8 T4
M98 P1003
/1 G55
M98 P1003
/1/2 G56
M98 P1003
M9
M99 (END MAIN PROG)
()
O1003 (PATTERN REPEAT SUB CALLS)
G65 P2003 E65. F30. U57 V58 X1.54 Y2.653 Z2.4
/3 G65 P2003 E65. F30. U88 V89 X3.21 Y4.0 Z2.4
/3/4 G65 P2003 E65. F30. U57 V58 X5.54 Y 2.653 Z2.4
/3/4 G65 P2003 E65. F30. U88 V89 X7.21 Y4.0 Z2.4
/3/4/5 G65 P2003 E65. F30. U57 V58 X9.54 Y2.653 Z2.4
G65 P2003 E65. F30. U88 V89 X11.21 Y4.0 Z2.4
M99
()
O2003 (NOTCH CUT SUB)
G0 G90 X#24 Y#25 Z#26
G91
#3004=2 (DISABLE FEED OVERRIDE)
IF [#21 NE #0] M#21 (COOLANT OPTION ON)
G0 X-.1
G1 Z-1. F#6
Y3.0 F[#5 * #535]
X-.1
G0 Z1.
IF [#22 NE #0] M#22 (COOLANT OPTION OFF)
G90 Z#26
#3004=0 (ENABLE FEED OVERRIDE)
M99

[mikenaturalice]

Maybe I flex my clicker muscle too much but I'd rather clickity click than whamity wham a machine on a lazy factor.  I don't even like transform but I will do it in the right application.  I prefer to copy a path and rechain.

Hmmm... different strokes, different folks and all that, but that seems odd to me. A couple jobs ago, we did 95% of our work on rotaries. The transform was sooooo easy!! Program a 'patch' of the part, transform/rotate around an axis, BOOM part programmed! 

I suppose it depends alot on what you program and HOW you program to make it usefull, but I thought the transform/rotate/mirror functions were the cat's xxxx. 

I am using hsm inventor at a PT job and it is such a pain to do rights/lefts and/or mirror images of parts/features. It might be int here somewhere, but after 10-12 years of Mastercam, I can't ever seem to find what I am looking for...

[jlw™]

Rotary is where I have used it in mcam.  Seeing Colin and Ron endorse it makes me change my thinking.  No offense meant to every one else.  I've been burned by it in edgecam.  More than once.  My fault for not giving it a go.  I rarely have the option of using it too tho.  Symmetry or repetitive features are uncommon.  Next chance tho, I'll giverago.

[Colin Gilchrist]

To be fair, I've been burnt by Mirror more than once. For Mirroring, I will always, always, use the "create new operations and geometry" option inside the Transform Toolpath. This takes more time, but you can be 100% sure that the lead in/out moves are correct, the cutting direction is correct, and no crashes are going to happen. Mastercam has improved Mirror over the years, and added features to eliminate the problems, but I've just never really trusted it after having so many crashes...

[JoshC]

Make sure to set the source to Geometry in transform for mirror, that will give you the "Reverse order" option on the mirror page, otherwise if the transform Source is set to NCI the Reverse order option will be greyed out and un useable.

[So not a Guru]

Can you transform a transform?  In other words, can I rotate a Finish Scallop and then mirror it?

Not only can you transform a transform, you can ghost the 1st transform. This is handy on occasion when you need to position a path prior to the transform you actually need.

[Jayson Kramer]

I am with Ron and Colin, I have used a lot for Horz work and 4th and 3axis for years. I have been teaching using the transform for many years at the schools I teach at.

Now I agree with Colin that the mirror option has been the one to bit me over the years. It is a better tool these days. I still am a little shy about using it at times.

Dang I remember using transform back in the early days a lot as I am acting like it was a really  long ago but V6 for mold cavities.

[Colin Gilchrist]

The last time I tried using Mirror, I had to make multiple Transform Toolpaths. As I went down the Operation List, I would make a transform for any 2D paths, and stop if there was a 3D path, create a new one for the 3D paths, and then another for any 2D that followed. I know they have been working on improving this over the years, but I still end up just creating new Operations and Geometry, as there are usually some tweaks that need to be made. I can see it working great for less complex parts, but when you are relying on it to properly mirror hundreds of operations, it becomes increasingly risky as the file gets larger. One of the big issues for me is that Mastercam is still a "Toolpath-centric" software. Each path exists on its own, without knowing anything about the kinematics of the machine. So issues like Travel Limits - both Rotary and Linear, and Fixture geometry aren't taken into consideration by the software. Sure, there are options downstream, once you get into Verify, but I still think the Mirror Transform could be much "smarter". Maybe I'm just paranoid, but I get total control by creating new Operations and Geometry...

[Fred @ Slate Industries]

I'm on 2017 and never going back but Funny how X3 / X4 Mirror  (debacle) still drives my transforming approach.

I mirror my solid ,geo  stock model and then use transform to verify it

But I still won't transform  / mirror it and then hit cycle start .

 

Back then I would send the reports into QC labeled

"I'm going to be Fired" !!

[AMCNitro]

Ive always avoided transform, I feel I have more control with copying and re-picking the new geometry.  But working in a mold shop it changes things, when a mold had more than one cavity its just easier(and faster) to just mirror the toolpath, it doesnt always work but when it does it saves a lot of time.  Its also not about being lazy, theres an older programmer that has been there ages and when he retires Id like to have his position in the office  , he uses transform a lot and I want to show I can program faster....  I asked because I dont have a lot of experience with transform.

[alexlikesyou]

I use transform all the time.  Most of the things I make have a feature that repeats 4 to 6 times so it cuts down on the clicking.  Though I always forget the specific settings when I'm using it to index the rotary and I end up with an unneeded amount of offsets.  Laziest way to mill wrench flats.

 

A few months back I tried tying it to a G68/G69 macro for non-rotary work but couldn't get it to post the correct parameters.  

[Fred @ Slate Industries]

2017 Transform / Rotate is bullet proof

4 Pallets 8 electrodes on each

Each electrode has identical detail every 120 degrees same ops each

 

Solo paths rotated 3 x per ghosting 1st set of ops.

Tranformed this ALL OVER THE REST OF THE PALLET and other pallet stations.

 

Still dont trust Mirror. Lol

[AMCNitro]

2017 Transform / Rotate is bullet proof

4 Pallets 8 electrodes on each

Each electrode has identical detail every 120 degrees same ops each

 

Solo paths rotated 3 x per ghosting 1st set of ops.

Tranformed this ALL OVER THE REST OF THE PALLET and other pallet stations.

 

Still dont trust Mirror. Lol

Mirror transform is the only one that gives me bugs, though not every time

[Fred @ Slate Industries]

I just finished a week of Transform / Mirroring with 2017

24 cores 12 Left 12 Right ditto on the Cav's

 

Mirror Knocked it out. (I of course verified the toolpath against it's solid model 1st)

 

Awesome.