[CMJacked]

Actually the mold is not complete, but for all practical purposes it is, I had one scare, when the finish tool moved from one pocket to the next, it did so at Z0, I fortunately touched it off on a .002 feeler gauge and left it there. I don't have a picture sharing site so I'm just attaching two photos.
I like the software to dollar ratio I'm getting with Bobcad. I thing it's a very good deal for smaller shops or even home based shops with very low overheads. Even though I use other cad packages I can see migrating to bobcad for a higher percentage of the programming I do. The tool control issue I have I'm sure I can overcome eventually but other that that I vote it a good deal for the money.

[moldmker]

Very nice.

Concerning the Z zero move, was your rapid plane set to zero?(check each operation)
If not, you may need to tweak your post to force the tool to the rapid plane between ops.
Would need more info to pinpoint area to look at.

Sounds like you already realize you probably just paid for your software by not sending this out to a shop equipped for 3d machining.

:cheers:
moldmker

[BurrMan]

Most of the posts have hard coded Z 0' in them that are meant to be worked with work offsets. If your just touching off, you'll want to get rid of these and just utilize the rapid planes that Mold mentions.

[Path]

Wow ... that is nice!

Can you tell us about what endmills were used.
Maybe the x, y and z increments (typical) to get such a smooth surface?

A few more in process pictures?

Great stuff .... thanks for sharing!


Path

[CMJacked]

Most of the posts have hard coded Z 0' in them that are meant to be worked with work offsets. If your just touching off, you'll want to get rid of these and just utilize the rapid planes that Mold mentions.

No The rapid plane is set to .1 all the other tooling moves used it well, even the finish mill made the retract plane in the pocket it was machining, The only move at Z-0-was the move between pockets. I dug into the code and there was a retract plane at that point but the next line sent it back to Z-0- before it made the second pocket position move. My work shifts did not have anything to do with it, the whole program would have been affected by any work shift discrepancy.

If not, you may need to tweak your post to force the tool to the rapid plane between ops.

That sounds more like it. I'll have to look into that.

I normally use Smartcam software, We spent over ten grand on the package and paid two grand a year support. Subbing out 3 and 4 axis work is not ever going to happen. This is not my first mold by any means just the first with this software package. I could not afford Smartcam at home. This is a very affordable option to me.

As far as tooling, The roughing was done with 1/2" HSS rougher, Semi finished with 3/8 SC BM at .12 step over and .1 doc, The pic feed on the finish mill (3/8 SC ball) was really coarse for a pic feed at .015, Normally pic feeds would start at half that but the machine I was running that job on only has top speed of 5,000 rpm which regulates feed rates, so for sacrificing finish for time I opted for a heaver run..

[moldmker]

If you launch the MillEditPost.exe utility (or notepad), you can search out your post and look at it.

But first, copy/rename the post so you can revert if needed.

Look under: Edit code blocks > Tool Change > Move to next cut same tool
In there you will see the variables used to output the G-code for that event.
zr is the variable that lifts tool to the rapid plane.

Sounds like you have something that's dropping the tool back down to Z zero.(I'm not sure what variable that would be.)
But it could be as Burr mentioned, see if there's a quote like this "G0 Z0.", that's a hard-coded move that could be deleted.

There must be something else going on, as well.
The drop should happen for all the tools, but you say it was only the finisher.
Did each pocket geometry have it's own CAM feature or did you select all 4 pockets for one feature?

You can also zip and upload your post here or let us know which post you're working with for more help.

[BurrMan]

The hard coded Z 0's are usually only in the "next cut, next tool" section, and not the "next cut, same tool" section.

FYI, usually there is one in the "standard start of program" section also, And the "end of program" section.

[CMJacked]

Great information guys, I will check that out today. I selected a feature for each pocket. The Z move was a feed move as well as the reposition across the mold face.
Where do you get a list of the strings and variables bobcad uses in their post? I have messed around with the processor engine but it's real basic. Like paint is compared to photoshop. I have used generic processors with another software product called Powerstation, They provided sample Marco's as well as detailed information on building processors from scratch. I thought that information was well guarded.
I'm not exactly clear on how everything works but I will enjoy learning.
My first post request to bobcad turns out to be a dud. Ezpath S control (conversational) with no can cycles. (Bridgeport) I've been back and forth trying to get arc's to generate correctly in a segment instead of full circles. Still no go. I've asked their post builder if he could provide me that info and no one has responded as of yet. The post is up for download on their site anyway full of problems.. They tell me everyone wants a processor with the can cycles ???? I don't know why. Size of programs is not an issue these days..

[BurrMan]

Go to the BobCad user forum. There is a thread there named post processors. In that thread there is a guy named sphillips who you can post the question to and ask for help.