Suppress Retract ?

[boro_boy]

Using a simple 2d contour toolpath with multiple chains, how do I get the tool to stay down and feed between chains? Tool insists on retracting and/or rapid positioning between chains,even with retract set to a value of 0[incremental] ?
thanks
Pedro, Socal

[charger19690]

Try putting your Top of Stock at your cut depth value, along with your feed plane.

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[boro_boy]

Originally Posted by charger19690 Try putting your Top of Stock at your cut depth value, along with your feed plane. Mike in MN

Thanks Mike, but I already tried what I believe to be all options, ie Uncheck rapid retract, use Clearance only at start/end of operation, set top of stock to 0[Inc] Depth 0 etc, basically everything logical but it still insists on retracting between.

[Superman]

The only method I know of is to join all the chians into one chain

[charger19690]

I know I got it to do it a couple times. When I get to work I will look up a program I did it to and get back to you, won't be till Monday though.

I just can't remember off the top of my head.

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[boro_boy]

Originally Posted by charger19690 I know I got it to do it a couple times. When I get to work I will look up a program I did it to and get back to you, won't be till Monday though. I just can't remember off the top of my head. Mike in MN

Thanks Mike, I'm sure there has to be a better solution, but for now as a workaround I saved the original multi-chain toolpath as geometry and then rechained as a single chain. I didn't think of this initially as I was trying to program the part efficiently .
thanks,pedro

[thebowman]

Originally Posted by boro_boy Thanks Mike, I'm sure there has to be a better solution, but for now as a workaround I saved the original multi-chain toolpath as geometry and then rechained as a single chain. I didn't think of this initially as I was trying to program the part efficiently . thanks,pedro

There is another alternative, Sir... I can't see calling someone I don't know boy, sorry.

In the Machining Operation Mangler right click on the operation you wish to change. Choose Toolpath Editor which is at the bottom. Step through the path and find the points that you need to change so you don't rapid up between chains.

I don't find Mastercam's toolpath editor to be very elegant or very intuitive. In addition, when you use Mastercam's toolpath editor you break the associativity between geometry and toolpath.

Both you and Mike might want to play around with Mastercam's Toolpath Editor and see if your opinions differ from mine.

[boro_boy]

Originally Posted by thebowman There is another alternative, Sir... I can't see calling someone I don't know boy, sorry. I don't find Mastercam's toolpath editor to be very elegant or very intuitive. In addition, when you use Mastercam's toolpath editor you break the associativity between geometry and toolpath. Both you and Mike might want to play around with Mastercam's Toolpath Editor and see if your opinions differ from mine.

bowman, thanks for the suggestion. Even more impressed that you somehow managed to get 'elegant' and 'Mastercam' to work in the same sentence

ps. Don't call me sir, I work for a living

[thebowman]

Originally Posted by boro_boy bowman, thanks for the suggestion. Even more impressed that you somehow managed to get 'elegant' and 'Mastercam' to work in the same sentence ps. Don't call me sir, I work for a living

Well, Sir with your approach I doubt you will ever be truly loved on e-mastercam.

I've read your posts here and I understand where you're coming from. In my opinion Mastercam isn't elegant and has many years to go before it ever might be considered elegant. On the other hand, I feel I have to know Mastercam cold because it dominates the machining job shop market and not knowing / understanding Mastercam would severely limit my job opportunities.

You might want to consider registering on Mike's Mastercam forum->

http://mastercamforum.com/index.php

if you wish discuss things like APT, why full control over the toolpath is really needed (a case like this is a perfect example), etc.

Please try the Toolpath Editor and let me know what you think.

Thank you in advance for taking the time to read my response... Sir! ;>)

[charger19690]

Originally Posted by boro_boy Thanks Mike, I'm sure there has to be a better solution, but for now as a workaround I saved the original multi-chain toolpath as geometry and then rechained as a single chain. I didn't think of this initially as I was trying to program the part efficiently . thanks,pedro

The link is a file that I did using multiple chains for a stick style program. I could have used transform, but I didn't...

Look at the Top Operation along with the Finish Profile operations. I was able to keep the tool down while rapiding to the next chain.

The trick on the Finish Profile was to have the Retract, Feed, and Stock planes "below" my Z Cut plane and then use the Clearance option with the check box turned on for "Before and After Operation".

I have also used the Toolpath Editor, but I normally only use that as a last resort because it locks the operation and if you make a change you have to regenerate it and go into the Editor again.

The file is X3-MU1. I know it will not open in anything before X3.

http://www.files.mastercamforum.com/NoRetractChains.MCX

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[boro_boy]

Originally Posted by charger19690 The link is a file that I did using multiple chains for a stick style program. I could have used transform, but I didn't... I have also used the Toolpath Editor, but I normally only use that as a last resort because it locks the operation and if you make a change you have to regenerate it and go into the Editor again.

mike / bowman thanks both for your suggestions. I think we all agree that the toolpath editor is useful but very clunky, which is a shame because I think it could be developed to be much more useful - Surfcam's toolpath editor is the best one I have used.
By the way Mike when you parted thru with the wheel cutter did the parts hold ok with that sliver of matl ?
thanks, pedro

[charger19690]

Pedro,

Yep held good. This was parted off with a Slitting Saw. On this project, these parts were 303SS, so it was pretty rigid.

I do this alot with small parts, trying to do with 1 operation like this. I normally try to leave .005 or .010 for the part to stay put. At the machine during setup, I normally have the operator/setup person play with the cutter comp to adjust for more or less material, which ever is the easiest for the thinnest amount possible that keeps the part on.

It's a nice strategy to make many little parts like this so you don't have to try to rip the stock off the back.

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com