Double Vise Redux

[chris m]

Having searched through the catacombs of the forum and talking to the reseller I still don't have a 'good' way to do what I wanna do. Here's the scenario:

 

I have a part that I am going to rough mill, 2 up, complete (two sides) in one op. I have 2 double vises on the machine with the long dimension of the vises along the X axis. The plan is to rough side one in the back vise and side two in the front vise. My issue is, for example, G54 X0 Y0 is right front and G55 X0 Y0 is back left since I want to be coming off of the solid jaw for both parts. I do not want to use coordinate rotation in the machine because my operators are very definitely not ready for that [personally I don't care for it much if it can be avoided]. I also don't want to machine part one, side one complete and then part one, side two complete which is what you get if you simply transform toolpaths with new geometry and then rotate one of the parts around. The only thing I can see to do is transform, then rotate one, then manually move each op to where I want it.

 

There has to be a better way

 

Or does there?

 

C

[Scott Reiner]

I think that what you want to try is the WCS. Oh do you have V9? If so you can use like the top toolpalane as G54 XY wherever, then set a new WCS and use G55 XY wherever.

 

HTH

 

Scott

[cadcam]

Chris ,I would do it the way Scott stated using the WCS..

Go to the mastercam site and download the V9 WCS view tut. here is the link to the page: WCS view location

this uses two diffrent vise's in two diffrent locations and one is g54 other g55 this will help you.

 

[ 09-24-2003, 11:00 AM: Message edited by: cadcam ]

[heeler]

Chris,

 

You can also use the C-Plane/Tool-Plane. We do this all the time. If you could send me the file I'll show you how I would do it.

 

Glenn

[chris m]

I use the WCS to get my origins in the right place but I still need to transform my toolpaths, then rotate the geometry created by the transform, then edit the WCS for each op (I wish they'd make edit common parameters actually work), then move the ops to where I want them.

 

Is this the only way?

C

[cadcam]

heeler,are we talking about using the Alt-O after picking Cplain or the other?

[heeler]

What we do is create a named view for each setup. Then make this be your T-plane/C-plane for your tool path. If you are doing the same part, but in different orientations, you just make a name view for each one. You can then copy each path and change the C-plane/T-plane. For example-use a clock face. We make the face of the clock in the top view with 12 in y+. We name this view SETUP 1 PART 1. We then rotate the view 180 deg. Now 6:00 is at y+. Mastercam will give this view a number. We will then name this SETUP 1 PART 2, We can then take the toolpaths and copy them and change the T-PLANE/C-PLANE to SETUP 1 PART 2.

 

HTH

 

Glenn

 

[ 09-24-2003, 12:16 PM: Message edited by: heeler ]

[chris m]

I put up a sample file on the ftp called 'Mill Transform Test.MC9' that shows the result I'm looking for but any better methods would be appreciated. Not a real part file, just something to play with.

 

C

 

[ 09-24-2003, 01:24 PM: Message edited by: chris m ]

[Chris Rizzo]

Hey Chris,

I grabbed the file and played for a while.... So you want to translate, rotate, change offsets, and sort by operations? It seems the operation sorting is the hang-up. How about doing the translation on each toolpath individually, and then rotating THAT translation...sorta like a transforming a transformation. When doing the translations, assign new offset (g55 here), increment 0. Then sort the whole bloody mess by operation type. Maybe?

 

I've got to get back to work here, and just sent my head spinning. Good luck.

[chris m]

cmr

 

Thanks for looking at the file

 

I actually want to sort by tool so that if I'm contouring and pocketing with the same tool it does all of the work on the 1st part, then goes to the second. Glenn emailed me a file [thanks Glenn ] that uses named views in an interesting way to accomplish what I was doing with the transformation of toolpaths.

 

This particular part is going to be a really good Mastercam learning experience for me. Thanks to all of you guys for teaching me some new stuff; any more ideas that you may have would be very welcome.

 

This forum is the cat's a$$

 

 

C

[Jeff from MLC-CAD Systems]

Chris, Im not certain if this is the same thing your talking about, but I had a customer that was running Bi-Lok vises and wanted his post to output

sub programs for all the parts cutting the same side of the part but he wanted the post to rotate

the back part coordinates so he could set his G54

work offsets on the hard jaw.

 

Simple solution "for me". I made hime a post that

buffered out all the motion then read it back in and added a simple switch to rotated the code for all the back jaw parts so what he ended up with was two sub programs one for the front part and one for the back part that had the code rotated 180 degrees.

 

I would contact my Dealer and inquire about this.

I think a dealer should have the resources to create or modify an existing post toa accomodate this feature. Im sure they wont do it for free as I didnt for my customer, but it works like a charm.

 

I also made the post support most all the machines they had since they really only wanted one post for all there equipment.

 

It is do-able. and its not that hard to do...

 

I agree the Transform that came out in what 7.1

has really not worked well for multiple part sub

ever and here we are on V9.2SP2 I dont understand why, but if the software wont do what we want we just make the post do it. It seems to be quicker and easier that the alternative. Everybody is happy...

 

Regards

Jeff

[cadcam]

Chris, just to let you know I got your mail last night and have not had any time to give it a peak.

 

I will thow.

[chris m]

Thanks guys

 

Jeff, I'm trying to decipher what you said about your post but it sounds very interesting. I don't think we're ready to shell out any $$ for post work right now, but down the road you never know. S4A is my reseller and 2 of those guys are out here often so I know that they don't have anything on the shelf like what you're talking about but maybe we can cook something up in the future.

 

 

C

[Jeff from MLC-CAD Systems]

Well Chris, Basically you program one part, then you use the misc settings to tell the post you want, lets say 8 parts then you also use a switch to tell it you want 4 of them rotated 180 degrees.

 

This will trigger the post to output multi part

sub programs one set for the front row and another set for the back row and all the calls

are in place in the main program the way they should be.

 

This particular post also has provisions for multi pallets if you want to run the second grab on another pallet in the same fashion.

 

This will have to do until they get the software to do these things correctly and this could take years or weeks depending on how important the developers thing these features are.

 

Later on down the line if you are interested and

your dealer isnt equipped to handle this let me

know. You know who I work for so getting in touch shouldnt be a problem...

 

Regards

Jeff

[McRae]

Chris,

 

Any resolution on this??

[chris m]

Not yet, been yanked off of this 'hottest job in the shop' to work on the new 'hottest job in the shop'

 

C

[crazy^millman]

Chisr can you use the transform rotate toolpath and use the subs to create the same effect. If you use the incremental offset shift from the orignal operation would this not create the first toolpath as a sub operation then the secone toolpat has a rotated toolpath with a offset 2 bigger than the orignal and Mpmaster suppoert these types of toolpaths very well. I have also had very good luck with the tranlate mirror toolpath and the rotate around a A axis. I have put this up here for you to take a look at.

code:

---

O9500

G20

G0G17G40G49G80G90

T14M6

G0G90G54P15X3.2Y.4999A0.S10000M3

G43H14Z.25M8

M98P0001

G69

G90X3.2Y.4999

G0G90G55G68X0.Y0.G91R0.

M98P0001

M5

G91G28Z0.M9

G28X0.Y0.A0.

M30

O9501

Z.03

G1Z0.F200.

X-4.F20.

G3Y0.R.25

G1X2.7

G2Y-.4999R.25

G1X-4.5

G0Z.25

M99

---

Dont know if that will do what you want but I did it with transform only with rotate and coordinate and used the origin as the control. I did a incremental sub.

 

Let me know kinda of intrested to see what you come up with.

 

Crazy Millman

[chris m]

Crazy

 

The problem with rotate is that rotated toolpaths [at least on my box] rotate the coordinate system and therefore post all of the X & Y moves the wrong way.

 

C

 

[ 09-30-2003, 07:38 AM: Message edited by: chris m ]

[crazy^millman]

Well I went back and reread your original post I can see I am going down a path you are not looking for. I will sit back from here and see what comes of it. I am trying to get you over to the dark side. That is just a joke.

 

Good Luck sorry about that.

 

Crazy Millman

 

[ 09-30-2003, 10:08 PM: Message edited by: Millman^Crazy ]

[Rekd™]

LoL, Millman

[crazy^millman]

Hey Rekd Glad soemone thought it was funny.

 

I have not talked to you in a while everything being going ok on your side of the 78. Been crazy over here but I did finnaly hire me some help he is green but they only guy I could find to work for the little money they wanted to pay.

 

Well if there is anything you need call me.

 

Crazy millman