Toolpath- Transform

[Candyman]

im still trembling with fear as to what could have been with the toolpath - transform option...in mastercam 8.1..

i machined a die block with a simple set of contours then all i wanted to do was to mirror the toolpath and thus machine the righhand die block but i twigged something was wrong when the mirrored toolpath would machine around my countor then rapid in z- my step amount then retract to z clearance plane then move to the next countour.. i thought ok its not doing any harm cause the rapid move is off the job so i watched the code line by line as it was executed.. then on the last pass at z-50. it machined the contour then it was going to feed right across my 50mm thick die block and go back to the start point again with a 50 mm cutter.. man i hit the stop button that quick it wasnt funny... anyway ive had this problem before but with edit nci its fine only thing is you cant reverse toolpath to continue to climb mill with the mirrored toolpath what gives here!!! any help thanks Paul

[Thad]

Paul,

 

We've had very bad luck with Transform/Mirror toolpaths. It's very buggy and unpredictable in my experience. When I get time, I'm going to prepare some files for CNC Software to look at. The mirrored path doesn't cut what the original path did, Reverse Toolpath doesn't reverse the toolpath (but sometimes it does), etc. I look over my programs very carefully when doing this and I always find something wrong. I hope to get it corrected soon.

 

Thad

[Jack Mitchell]

Mirror imaging will change the following:

 

G02 becomes G03.

G41 Comp left becomes G42 Comp right.

I, J, K, vectors will change the signs dependant on the mirror of "X", "Y", or "Both" axis.

In the case of mirroring along "X" all signs for the "X axis will change as well.

And of course, Climb milling entertains conventional milling.

 

Mirroring has sucked ever since its inception - but alas, it's math! NOTE: This opinion refers to mirroring and not Mastercam's product or procedure.

 

The primary need for me was aerospace machining, the largest argument was climb milling all to a desired finish. - ultra large when doing tapered walls with blended radii at every edge.

 

Mirroring in Mastercam is relatively easy and well worth the lessons learned. Please upload to Jayson's FTP and we might be able to observe and suggest an attack to avoid future problems. Please be specific with the upload and location in your response.

 

Regards, Jack

 

[ 07-12-2003, 02:22 AM: Message edited by: Jack Mitchell ]

[mold100]

I would normally mirror the geometry then regen the tool path then I could control it, I would

always need to reverse any chains for correct cutter path.It sounds like more work than it really is.

[BernieT]

I've had good luck in mirroring toolpaths in both 8.1.1 and 9.1. Especially finish surfacing.

 

'Reversing toolpath' requires careful checking, sometimes the situation just doesn't allow reversing. Mostly when you have stepped depth cuts or ramped contour toolpaths.

 

Just last week I had an instance where I tried to mirror a finish surfacing program in the Centroid control and it bombed (G19 arc - in graphing, thank heavens), went to MC and 'Transform - Mirrored' reposted and it worked fine.

 

Thad, sending a representative sample to CNC is a good idea, it would be nice if they could cover more situations with mirrored - reversed toolpaths.

[Thad]

quote:

---

'Reversing toolpath' requires careful checking, sometimes the situation just doesn't allow reversing. Mostly when you have stepped depth cuts or ramped contour toolpaths.

---

BerTau,

 

How so? The help on the Reverse Toolpath box states that its function is to allow you to continue climb cutting even though you're mirroring the path. That's pretty cut and dry. If I still want to climb cut, I check it. If I don't, then I don't check it. The problem is, when I check it, it still conventional cuts! That's just plain wrong.

 

Thad

[Fig sign]

Have a look ,plz!

 

Iskander s!z Sorry for so short answer , I am in hurry !

[BernieT]

Thad,

 

I guess I haven't run into that situation in ver 9.1 yet. You are right - that is just wrong and should be fixed.

 

quote:

---

It's always worth a shot to try it though...for me anyway.

---

Reading that previous thread made me realize that is exactly what I do - try it, it's quick, if it works great, if not find another way. Mirror-reverse has never been completely reliable but I tended to blame it on all the variations of toolpathing rather than consider it a bug.

 

I'll try to pay more attention from now on.

[cadcam]

You guys could put these problem files in the folder files For CNC Inc.

Then CNC will have a backup to of what you send them.

[Thad]

Good idea Jay. Right now, there are too many hot jobs in the shop. Going on week 4 of 11 hour days. Hope it lets up soon!

 

Thad

[Müřlıń®]

Paul....What I do when I need to do a right and a left hand part is:

 

Mirror the geometry, then regen the toolpaths.

 

It gets a little trickier if they are both in the same block though.....

 

 

Murlin

 

[ 07-18-2003, 07:42 PM: Message edited by: Murlin ]

[Thad]

I've got some "free time" so I uploaded a simple file to Jay's FTP called MIRROR THAD.MC9. It's in the V9 files folder.

 

I did a 2D contour around a simple shape. In the transform parameters, I selected Mirror and Create new operations and geometry. On the Mirror parameters page, I checked Y axis, unchecked the View box and checked Reverse Toolpath because I still want to climb cut.

 

I left the mirrored geometry as the result color. If you backplot these, you'll see that the original path climb cuts, but the mirrored path conventional cuts. With "Reverse Toolpath" checked, they should both climb cut.

 

I will put a copy of the MC9 file in the CNC Software folder and email it to them as well.

 

Thad

[Marty A]

hey there thad

i pulled your file and looked at it. i then reversed chain and it looked to be fine. am i not seeing something here or am i just an idiot.

 

marty

[Thad]

Marty,

 

The first toolpath is the one that I programmed. The second is the result of using the Toolpath, Transform option to let Mastercam mirror my program for me. If you right click in the Ops manager, you will see these options.

 

You are right, reversing the chain will work fine. I want Mastercam to correctly mirror my toolpath without having to mirror my geometry and reversing the chain (like you do it.) When it works, it's a great time saver. You should try it.

 

Thad

[Müřlıń®]

My bad, you guys were talking about contours, I was talking about surface toolpaths.

 

I must pay closer attention....

 

 

But I think you guys found a use for the reverse toolpath toggle

 

Perhaps that "was" the fix for mirrored contours??

 

I had the same problem back in Ver 6 when I would try to use Edit NCI to mirror complex 3-d surface models, it never worked.

I just got in the habbit of mirroring my geometry since it seemed to solve so many other problems

 

 

Murlin

[Marty A]

hi thad

i see what you mean now, i'm going to play with that today since i'm not real busy.thanks for the info.

 

marty

[Thad]

Murlin,

 

I get the same results when doing a surface rough pocket. I just used this 2D contour as a quick and easy example.

 

Thad

[Thad]

Marty,

 

What I do now is leave the View box checked and don't check the Reverse Toolpath box. This gives me exactly what I want.

 

Thad

[Marty A]

thad

 

i'll try that. i'm trying to miirow my part like you had but with no luck. help wasn.t to clear for me. some thing about the parameters.

 

marty

[Marty A]

thad

 

ok thad i'm starting to get this but it still isn't climb cutting.

 

 

marty rather be bass fishing

[Müřlıń®]

Thad....If you mirror your geometry and then regen, won't you still be climbing on all toolpaths that dont require a chaining direction? Works for me to keep climbing. But I use mainly surface toolpaths.

 

Surface/rough/pocket uses a direction for the finish cut. So if you just mirror the NCI, it will have a reversed finish path.

 

Using a complex surface model with 35 megs of toolpaths on it only takes me a short time to regen. Mirror geometry, select all in ops, and hit the regen button. Go get a cup of java, flirt with the office ladies, shoot the bull with a couple co-workers. Come back and its done

 

Murlin

[Zero]

I've also had good luck with mirroring toolpaths. I never select create new geometry and paths, as this nullifies the whole reason you're mirroring in the first place, to save time, and tons of it I might add. Granted, climb/conventional makes no difference to me, as we dont really cut any metal or anything else that hard and everything done on the machine always gets sanded and painted, so I don't pay attention to these minor details . I did have a little trouble at first when we switched from 8.1.1 to 9.0 mirroring with different wcs', but I'm not sure if that was me or the system....everything seems to be working hunky-dory in 9.1sp1. It is a little buggy though,, so you have to watch out for reversed arcs and such that go the wrong way and can cause some pretty bad gouges, but thats what backplot and verify are for....

 

JM2C

 

[ 08-05-2003, 09:19 AM: Message edited by: Zero ]

[Thad]

Murlin,

 

I'm familiar with a few workarounds. That's not the issue. I'm pointing out that the Reverse Toolpath option doesn't reverse the toolpath.

 

Thad

[Zero]

quote:

---

Using a complex surface model with 35 megs of toolpaths on it only takes me a short time to regen. Mirror geometry, select all in ops, and hit the regen button. Go get a cup of java, flirt with the office ladies, shoot the bull with a couple co-workers. Come back and its done

---

This is what I mean (no offense intended Murlin ) by not mirroing geometry. Without creating new geometry checked, those 35 megs of mirrored toolpaths are generated in about 10 seconds (if that) instead of well...however long getting a cup of java, flirting with the office ladies, shooting the bull with a couple co-workers, come back and its done takes

 

[ 08-05-2003, 09:23 AM: Message edited by: Zero ]

[Müřlıń®]

Zero, yes if you are only needing the fastest way to generate a toolpath, you are right

 

I must STL compair everything to be 100% sure there are no little surprizes.

 

Picking my way thru 60 toolpaths in ops, is a little time consuming and error prone. Especially if you get interrupted alot.

 

When I upgraded to VER 9, I got 3 jobs back to back that required me to make right and left-hand parts.

 

Mastercam made it soooooo easy.........perfect every time.....

 

 

Murlin