Can Your CADCAM system do this?

Lets say you have programmed a "left hand" part with 20 operations. You now wish to program the "right hand" part and mirror the toolpaths
and then transform them for 3 vises (G54, G55, G56). The only way I can do this in Mastercam X2 MR2 SP1 is to mirror each toolpath individually (that would be 20 mirrored toolpaths) and then transform all the mirrored toolpaths. What I would like to be able to do is to mirror all the toolpath at once and transform them rather than being forced to mirror each toolpath individually (in this case 20 times.).
I've tried to do this with no luck in Mastercam.
I'm told I can't do this.
Can your CADCAM system do this?
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
jon_banquer wrote:

Not the answer you're looking for I'm aware so I'll probably get flamed for this, but that is what sub programs are for, Jon.
Mirroring toolpaths is generally not a good idea anyway, Mastercam doesn't do a very good job of it. If you want to maintain climb milling when contouring you need to mirror and reverse the toolpath. Acu-Carv had that perfected. However, mirror and reverse a roughing path and the last pass gets cut first. Oops! If you're programming with cutter / wear comp, you're in even deeper shit, Mastercam will start switching left / right - G41 / G42 at random. Good luck with that.
Mirror your geometry, copy your operations and reselect the new geometry.
For using different fixture / work offsets sometimes I use Manual Entry. It is even less work if you modify the post to remove the parentheses around the manual entry in the posted code, you won't have to edit the code to remove them. Especially useful for 1GB+ surfacing programs. :)
--
Black Dragon

The United States Army:
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Flamed from whom?
Me?
Not a chance.

Our shop uses Wear comp as a standard. I'll look through the code and see if I can find any reversal of G41/ G42. Thanks for the heads up on this.

Rechaining 20 operations takes time. I'd like to save this time.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

To do what, exactly? Publish more? Put more glob on yer Glob?
--
PV'd

>
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

How about saving the file as a "right hand", and mirroring your geometry? then regen all toolpaths, you may have to go into your geo and "reverse" the chain, but you will still have native geometry to work with.
The time it should take to do this would be less than 1/2 hr.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On Sep 13, 11:53am, snipped-for-privacy@msn.com wrote:

You know I didn't think to try that. Would be a great solution if it works.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

You know I didn't think to try that. Would be a great solution if it works.
***** There is a minor issue with that, mastercam sucks when you regen a bunch of ops after mirroring the geometry. Make a transform/mirror op, switch the reverse toolpath box, all will be fine.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Only way to know is to try. I haven't tried what's been suggested yet. I like trying new stuff like this. Only way to find out what works and what doesn't. I appreciated his suggestion. If it works fine. If not I still learn... maybe more if it doesn't work.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Mirror the geometry and regen the toolpaths...new stuff? (use the ops page man!!! Never redo work thats been done already) lol
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
> Mirror the geometry and regen the toolpaths...new stuff?

Not new at all. I figured why bother to mirror the geometry. Why not just mirror the toolpaths and transform.
I think it has much more to do with understanding what Mastercan can do well and what Mastercam can't do well.
Perhaps asshole Brewer will come along and say just read the help manual. Try learning how to use Change At Point using the Mastercam help manual or the Mastercam Reference guide... it ain't there. See my thread in the e-Mastercam forum on Change At Point. Brewer's too stupid to read it and understand it. You're not.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Select all the operations needed, right click, make a tranform op. In the op check the checkbox to reverse toolpath.
Acu-Carv

That's the best way.
main program...
G54 M98P1000 G55 M98P1000 G56 M98P1000
or, you could change the misc value to G55 etc... for the first op of each piece after you transformed them.
I would make 3 groups. in each of the three groups add a tranform op and mirror all ops. Then in each group change the first op to G58 or whatever each one is going to be. And remember to switch the reverse toolpath in the mirror page. (but I suggest the main program gimmic, it's just too simple)

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

The shop doesn't us subroutines. I think the reason is that we have an issue with our post that needs to be fixed. I'll get with my boss and our VAR on this. Maybe this week. No way do I want to us separate subprograms and have 20 separate programs. All in one program or nothing. I'm still unclear how subprograms work in Mastercam as I haven't used them yet or exactly how to set this up and make it work.

No. I don't want to do this.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

The shop doesn't us subroutines. I think the reason is that we have an issue with our post that needs to be fixed.
hmmmm. Maybe your sub proggs are too complex? I'll use a haas example cause thats what I use now, but all machines are basically the same. In a haas the main program is nothing more than
G54 P98M1000 G55 P98M1000 G56 P98M1000
1000 is the program name. Those three lines are the "complete" main program to run in three vices. program 1000 is made in mastercam. It cuts one part. At the end of program 1000 add a "G99" thats it. (adapt to whatever machine is being used)
Shit...If it gets easier than that..Ill invest in it.
I'll get with my boss and our VAR on this.
"screw both those idiots."
Maybe this week. No way do I want to us separate subprograms and have 20 separate programs.
**** no, your misunderstanding me, One program out of mastercam to cut one part. A main program runs the mastercam program. The main program consists of only three lines for the vice offsets. ************
All in one program or nothing. I'm still unclear how subprograms work in Mastercam as I haven't used them yet or exactly how to set this up and make it work.
Screw mastercam and subprograms. Do it in the controller...three lines?

No. I don't want to do this.
(I would suggest against it, make a main program in the controller with three lines to run the 3 vices. Otherwise mastercam will spit out three times the code needed, and that takes loger to load than writing a 3 line master program in the cnc.)
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Unless, you wanted to do it right. Each tool complete in all three vices before getting the next tool. In that case I would program the part, say it has 20 ops. Then select it all and make a transform/mirror op with delete the old ops selected and the reverse toolpath checkbox set. At this point I would grab all the ops I want for the first round of 3 vice cuts and drag and drop them twice. Then edit on the first page of each op the misc button, set the first line to G54 or G55 or G56 etc...
Do that for each tool.
Will take a few minutes, but now all tool one will run all three vices before getting tool 2, the tool 3, etc... lots more efficient.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Of course that's what I'm doing.

Suggest you go ahead and try what you wrote above in Mastercam X2 MR2 SP1. It doesn't work which is what I said in my first post. Please go back and read my first post again. You have to mirror *each operations toolpath separately*. Only then can you transform all the mirrored operations. IOW, Mastercam will only allow you to transform mirrored toolpath if they are separate operations and not together. Try it and you will see what I mean. Make sure you post it out.
No way in hell am I going to manually change all the toolpaths to G55, G56, etc. If I wanted to do that I'd use OneCNC Crapware.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
jon_banquer wrote:

I really haven't heard of any cam software that would do what vinny said out of the box.. it would probably take a nicely edited post and some finessing with the operations to get exactly what you want.
sometimes when your setting up for multiple fixtures, running production jobs, you just have to bite the bullet and write/copy/paste a program yourself. The way vinny said would be the best..
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Only if you have a CADCAM program that's a P.O.S. or you don't have a handle on how to do a workaround in your CADCAM system.

What did Vinny say would be best? Be specific.
alt.machines.cnc isn't CNC Advertising Zone and your unmeasured crap doesn't fly here. There also isn't a moderator and an unscrupulous owner to back you up and coddle you like a baby.
Jon Banquer San Diego, CA http://jonbanquer.blogspot.com /
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Jon, Tell us how it worked out, what you did to get the right hand part done. Did my method work? I did a basic part in V9.1 and had to reverse toolpath and change side on contours only, pockets stayed as they were done on left hand part.
Let us know
"D"
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Since we are on a mastercam kick...I have a question. I'm looking for a Mastercam 9 answer or a generic answer telling a way in any cam system. I think there is a toolpath specifically to do what I want in X, maybe its called notch cutting or slot cutting, or something like that. But anyway I'm in 9.1 and what I am doing is cutting a runner for a mold. Its nothing but a slot cut with a form cutter. Lets say the slot is .25 deep and 6" long. What I do now is grab the centerline and make a copy at Z-.250. Then I make a ruled surf with the 2 lines and tell the system i'm using a .0001 cutter so it wont offset to the side.. I do the ruled surface because I want to cut back and fourth, stepping down say .005 at each end. I know ramp will do this, but I dont want to ramp. If I select the geometry and make a chain back and fourth it wont go down at each end, and I dont want it to rapid to one end each time, thats why the surface as opposed to a contour. When this is done I usually make a contour .001 off center each way so I can make one pass at the end climb cutting for looks. And this works fine, But just in case I'm being an idiot and there's a specific way to do this. It seems extremely common, makes me feel there's a better way??
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Vinny, I created one 6" line at z-.245 and y.0001, and another at z-.250 and y-.0001, connected lines at one end with 3d cplane, ran 3d contour at . 005 step down per pass. Each pass produced .01 of depth cutting, back and forth,,,,,,, comp off, no lead-in / lead-out, keep tool down.
"D"
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.