[Vigilance]

Has anyone tried to run a Gerber Sabre 404 router with Bobcad-cam? I have a full sheet specifying the relatively few G-codes it will accept (seems they crippled the machine so that it will only run 2.5 axis for G-code). However, I know that the machine is fully capable of 3D. I know this because Gerber has an "Autocarve" feature that will cause ramping for square corners - a 3D move. Also, Cimigraphi worked on the machine in full 3D by using Delcam's "Gerber spooler" (I can't find the HASP to run Cimigraphi anymore, though).

How do I interface Bobcad with the machine for full 3D use? Sure, Bobcad's tech department says they will come up with a post processor to run the machine, but I have a feeling they will only do G-code, which will only run the machine 2.5 axis.

My idea is that, if nothing else, maybe Bobcad's post can be configured to feed Delcam's Gerber Spooler, although the code is odd to say the least. Anyone have any ideas?

I can provide samples of the code generated by Cimigraphi's post processor to feed the spooler, as well as the script used to run their post processor.

Thanks,

-John
:withstupi

[tjones]

Post the examples and just maybe we can do something for you.

[Vigilance]

Seems that it wont let me post them here. I will email all the information I have to anyone willing to help.

I have three or four files that should be useful. One is a sample of Gerber code that is used to cut a series of 10 rosette blocks (pattern only). Another is the spooler itself. The other two files are Cimigraphi scripts used in the conversion. One for generating Gerber code, the other used for ISO G-code. I think the two scripts side by side might do the most good.

My email is [email protected].

-John
:violin:

[Vigilance]

Here's a sample of code that will run the machine - however, I don't know how to vary the spindle rpm and other important functions.

#R4000
#R4100
#R49000061A8
#MJob Start. Load Matl
#R4101
#R4001
#M1:Tapered Flat H0.25 A45 D0.01 <20000 R.P.M>
#R4A00000001
#F100
#P100
#D0.84200 0.84200 -0.25000
#C0.84200 0.84200 0.18160
#B0.84200 2.78300 0.18160
#B0.65600 2.96900 0.00000
#B0.84200 2.78300 0.18160
#B2.78300 2.78300 0.18160
#B2.96900 2.96900 0.00000
#B2.78300 2.78300 0.18160
#B2.78300 0.84200 0.18160
#B2.96900 0.65600 0.00000
#B2.78300 0.84200 0.18160
#B0.84200 0.84200 0.18160
#B0.65600 0.65600 0.00000
#B0.84200 0.84200 0.18160
#D0.84200 0.84200 -0.25000
#D-0.06240 -0.06240 -0.25000
#F100
#P100
#C-0.06240 -0.06240 0.24420
#B3.68760 -0.06240 0.24420
#B3.68760 3.68760 0.24420
#B-0.06240 3.68760 0.24420
#B-0.06240 -0.06240 0.24420
#F1000
#P1000
#B-0.06240 -0.06240 -0.25000
#B0.00000 0.00000 -0.25000

Seems simple enough, but it gets really confusing to me. This is one of the programs we generated with Cimigraphi's post processor. F seems to be the XY feedrate, P seems to be the Z feedrate, B seems to be for standard moves. The D and C functions I have no idea (but it screws with the machine if they are replaced by B - maybe they are specific rapid moves?). The R commands seem to each have more than one function each, (i.e. menu item plus disable spindle and z axis). In our old Cimigraphi sheets, they highlighted the #R4A00000001 as "depthcalc". Placing a #M anywhere results in a pause, and it will display anything immediately to the right of the M. This means that the <20000 rpm> in the above text is just that - a displayed string, not a speed command. The spindle seems to be running at about 20000 rpm by default, no matter what I put in the program. Also seems that since M pauses it, that's what normally passes for a tool change (no ATC).

I'm continuing to play with it, but I'm short of ideas by now. #N doesn't seem to do anything, and #T is read as an error by the spooler. I wish I could see the files being passed to the machine by Gerber's software.

-John
(chair)

PS - I called Delcam - talked to 2 people - they stonewalled me - no information. (nuts)

[Techmachineman]

I would call and make sure you actually speak to a tech guy. Many sales guys alot of times claim to be tech to make the sale. Just be sure they write you a post and let you try it before buying. You dont want to pay alot of money out and just hope for the best from a "money back guarantee they offer". For more information on that, see thread before, "Beware of Bobcad 2".

[Vigilance]

To my knowledge, they won't let you output anything to a machine (or write a post) without you buying it first. I guess that it's irrelevant now, though, since we already purchased it.

It seems like no matter whose tech department I talk to (Gerber, Delcam, Bobcad, etc), no one wants to talk to me. The people at Bobcad seem to be really angry though, and I have no idea why. I spoke to a man named Ed in their tech department, and he said that if he had a sample of the code we sent to the machine with Cimigraphi, they could write it. Kind of a bold statement, but who knows? Maybe they'll pull through. I don't know if that sample code I gave them contains any spindle rpm information or any of that, so it will be interesting to see what they come up with.

I trapped (and logged) the data sent to and from the machine through the serial port from Gerber's software, but it's in ASCII and raw hex. Don't know if this is going to help much, but it's all I have besides the aforementioned files.

The folks at Delcam claimed they don't know how the machine works, but how the heck would you get the machine to run without knowing how it works? I trapped the data between their spooler and the machine as well, for comparision. I know they're lying to me, but hey - I didn't buy their software, so why would they care?

I'll try to keep everyone posted, and if anyone has any ideas, please let me know.

-John
[email protected]

[Techmachineman]

In my opinion, I don't think it will work. This is one of the reasons why they should let you try it first. Because if it doesnt work, then you'll get the run around and get only partial refund.

[Vigilance]

Ok everyone, here's the files (now that I think I know how to post them here). There is a data view and a request view of the serial data (consult the request view if you'd like to examine the most detail, including matching the ASCII text to the raw hex. Also, there is a file name "test code for gerber - trial 2.txt". The original extension is .ger, but it's plain text. Also is a file I made from my examination of the ASCII and hex, compared side by side with the code text input to the spooler (gerber spooler - trial 2 - breakdown.txt). I made the code intentionally repetitive so that I could find patterns in the code that relate to functions in the text (I hope I haven't lost anyone).

Hopefully this data will be helpful - it has taken me several work days already to format and interpret this stuff.



Does anyone out there own ArtCAM? If you do, PLEASE post a few simple Gerber files for me. Nothing complicated for now. Just have the router do a rectangle or diagonal move, and maybe a ramp move, then return to start. Also, please make more than one post, and ONLY change the spindle rpm between posts. This will help me find the spindle RPM function on the text side of the spooler.
You don't need a Gerber router to do this, just have the program post to a Gerber formatted .ger file. This would be greatly appreciated.

Thanks.

-John
:idea:

[tjones]

Looks like quite a bit of work to modify your post. I think starting small would be the best. Is there any existing posts that could come close?

Have you checked in the support for existing posts?

[Vigilance]

I've checked into all of the Bobcad posts that I thought might help, but nothing close to this code. I have different ideas though.



Sorry I haven't posted in a while, but we've been horribly busy at work (I am day labor as well as being a CNC operator)

I've figured out what has been passing for a "post" for Cimigraphi. They wrote probably the sloppiest hack I've seen so far for an input to the spooler (uses only one motion type that I can tell (linear 3D) and doesn't even control the spindle RPM!), which indicates to me that they probably stole it. :nono:

Does anyone know which Bobcad post is generic, plain, un-modified (aka STANDARD) G-code?

Thanks.

BTW, no longer need the ArtCAM posts.

[tjones]

a basic fanuc would be it

[Vigilance]

Which is a "basic" Fanuc, though? I see a lot of different posts for Fanuc machines on Bobcad's support site, so I am a little confused. I have downloaded several Fanuc posts though, (Fanuc 3000C, Fanuc 6M, Fanuc 20F manual tool change, and Fanuc (all comments). )

Are any of these the one I need?

Also, does anyone have any ideas on converting a G-code specified curve into a series of tiny linear segments? This Gerber machine does not appear to be capable of normal circular or parabolic interpolation, not even in 2D. Their software appears to break a curve down into small linear moves - on a half circle (5 inch radius) the software broke the arc down into linear segments approximately 1/8" in length. However, when machined, curves are generally very smooth - they are not choppy. This must mean that for smaller curves, the segments are probably shorter, and the smooth arc must result from the acceleration of the axes.

What I don't know is how this is calculated, or how to generate that series of linear moves from a G-code command. Any ideas on this? All I need to do is take a curve command, such as a G02, G03, G06, G72, or G73 and convert those moves into a series of x,y,z moves.

Also - I need to invert the Z-axis. This machine reads it's Z moves as a depth measurement - not height. Positive Z values go down, negative values go up. Zero Z height is the top of the workpiece.

This is one of the last pieces of the pie here, folks. Once we get this figured out - I might be able to run this thing.

:banana: We're really close here!

[smurph]

Oh boy... This will spell the end of what you can do in the BobCad post processor. You are going to have to run the G code output of BobCad through another "conversion" program.

If you are going to have to create your own arcs, then it doesn't really matter which post processor you use. Just pick Fanuc 6M and copy it to a different name.

You will need to modify most any Fanuc based post because calculating the arcs will be easiest with absolute midpoint coordinates. Fanuc uses incremental arc midpoints. Change the arc midpoints to be Absolute. For the canned cycles, uncheck all of them. BobCad will generate the long code for the canned cycles if you mark the post as not having any. (Pretty damn cool thing you did there BobCad!!!)

Now, about creating the arcs... What programming languages do you speak? I have some VB code that I wrote to make a back plotter. I scrapped the project because there was a nifty link on this board (in the vb programming section) to a nifty back plotter in VB 2005 that was a little more advanced than my efforts. But my humble code does just what you want it to do. It draws a circle with many little lines. That's because you can't really draw a real arc using GDI on a window! So in effect, it will be perfect. Well... almost. it just needs learn to read G02 and G03 inputs and to spit out X, Y, Z movements instead of screen drawing commands. But the arc segment calculation is there. I spent several weeks perfecting the little devil. It made me wish I had paid more attention in geometry/trig classes!

So in my mind, what you will have to do is make a very vanilla post processor in BobCad that uses absolute coordinates for the arc midpoints. Then create a new "post post" processor/converter program that takes the vanilla G code and spits out your Gerber code.

Let me know if you want to pursue this route.

Steve

[Vigilance]

That is exactly the route I plan to take. :devious:

As far as programming languages, though - I'm ashamed to admit that the last thing I programmed was a TI-89 calculator! I think those use at least some form of the Basic programming language though.

The arc segment calculation code you have will probably prove to be most valuable. Also - do you have any code to convert a decimal number to hex? :withstupi I will need to be able to do that to make everything work nicely. I know that sounds absurd, but I will have to feed some raw hex through the spooler to get the nicer functions to work.

One question I have though - why absolute instead of incremental? I have to check again, but I believe the only thing absolute is used for on the router is for the home position - but again, let me check this (I'm probably wrong). I also have to do some investigating to see how the thing deals with negative numbers (probably not an issue anyway, since the spooler does a fine job with this).

I am hoping to write the converter so that it uses a "standard" G-code file - that way, I don't need to mess up whatever Bobcad (or any other program) is putting out normally. Scott Phillips (I think that was his name) over at Bobcad told me the Fanuc0M was the most basic G-code post.

As far as canned cycles - I don't think the machine really has any - but, since I'm not going to be doing any threading with a router, I don't think I have much to worry about .

When this gets put together, I think I'll post a video - this will certainly be something to see.

[smurph]

I don't think there is any code to convert a decimal number into hex. Where is the decimal in hex? Or do they just represent the decimal number (float) as it is in memory? I need some examples, I guess. Like what would 123.456 look like in the hex format that goes to the router?

Steve

[Vigilance]

2 inches would be sent as 00 03 0D 40 for an individual measurement (all measurements are 8 digits or 4 bytes of hex).

00030D40, converted to decimal, = 200,000 = 2 inches, in this case.

I can send you an email, explaining more, but this is the basic format of it.

Just take your decimal measurement, say 2.00000, and multiply by 100,000, then convert to hex. Took me some frustration and a lot of time to figure this out, but it works perfect.

[smurph]

Ok, I think that is just the binary representation of 200000 in big endian. This is what goes in the serial stream to the router, right?

Like you said to email me. Or give me a call.

Steve

[Vigilance]

Sorry I haven't gotten the chance to email or call, yet. I'll call or email ASAP, but it probably won't be this weekend (I'll explain later).

Thank you for being patient with me.

-John