Questions???

[termite]

Has anyone thought of putting a writing instrument into the bot? I do not want to cut foam in my shop (the mess). I have been doing practice cuts in plywood (expensive). I was thinking of attaching a pencil (this is a plotter) somehow but do not know how. Does anyone have any ideas? I am new to this and am learning every day and trying to teach the bot to high school students. It has been interesting.
Other questions. How do I do raised lettering? I am using autosketch as a cad.
I was at New Orleans with shopbot and they had a sign there that the cuts were of varying depth on the individual letters like tombstone carving. I was told that cassmate software did it. That is too expensive for me. How do I do the varying depth. I already know about individual lines but do not want to edit each line in a converted program. Is there another way?
How does anyone do multiple copies of the same thing in one cutting?
I have more questions but this is enough for now.
Thanks for your help
Bill Lindsay

[rgbrown@itexas.net]

Bill,
Some use a felt tip pen in the router chuck to trace the path. An adapter might need to made to fit the router or, one could run it on the tool carrier with a holder on an offset.
TurboCad has a free download and tutorial on their website for a 2D CAD program. I know of no 'inexpensive' program that allows 3D draftng and conversion, though there is probably one out there.

Ron B- rgbrown@itexas.net (mailto:rgbrown@itexas.net)

[studio@renc.igs.net]

I have been working for over a year to get Casmate
to router the very sign you saw. It still is not working. The sign you saw had flaws in it.

Richard

[john@pcjet.com]

Has anyone used Mastercam? I saw the results of some of the work and it looked pretty good.

John
J.E.T. Enterprises
john@pcjet.com (mailto:john@pcjet.com)
www.pcjet.com

[arthur_ross]

I'm using CorelDraw to create the lettering, exporting as HPGL to ScanVec Enroute, and use Enroute to create the fancy 3D carving effect. The folks at ScanVec were great about creating a postprocessor to output G-Code from Enroute.

Enroute is expensive (about $2500), but that or EngraveLab are the only two programs to create 3D paths for the "handcarved look" (unless you go Gerber, and that's another story....)

Arthur
Deltamation Inc./www.signsontap.com

[dale]

I have been using Mastercam for about a year now. It has saved me countless hours. I have been making placques that are oval in shape with a 1/8" deep pocket. Inside the pocket is raised lettering. Mastercam can write the program in about 5 minutes. Bruce's G-code converter takes another 30 seconds and I am ready to cut it out.

I have just started working with 3D surfaces and the possibilities seem endless.

Mastercam is a good tool.

Dale

[bruce_clark]

Mr. Ross:

There is another program that will give you the
"hand carved" effect. That is AlphaCam. Nice
program, though the entry level version
AlphaEngrave is ~$2500.

I used it to engrave a celtic design cross on my
SB (and to help debug the G-code converter) and it
did a nice job (for the first ever try).

You can find more information about AlphaCAM at
http://www.licom.com

Bruce Clark
bwclark@centuryinter.net (mailto:bwclark@centuryinter.net)

[arthur_ross]

Bruce-

Thanks for the info- can you post or e-mail a pic?

I've done some preliminary work on a low cost program to generate G-Code for V cut lettering for a couple of fonts- I'll finish it up if anyone's interested...

Arthur
Deltamation Inc./www.signsontap.com

[termite]

Richard the sign still looked good to me!!!! I would like to just achieve that level.

[gberscht@sk.sympatico.ca]

Bill,
To attach a pencil to your router is very easy.
If your router uses a 1/2" shank all you have to do is take some 1/2" doweling and cut it about 3" long,if you are close to a hobby shop pick up some nirod,it is used on rc aircraft to move the control services,try and get the biggest you can it comes in different colors I think blue is the strongest.what this does is one tube slides inside each other.now bore a hole the same size as the outer tube of the nirod ito the doweling.Dont bore all the way through,leave about an inch,next talk a spring out of a pen and put it into the dowel,slide the outer nirod tube into it you may have to glue it in place.Now take the inner nirod tube and slide it into the outer tube so that it hits the spring,cut it to the right length,take a lead from a pencil and press it into the end of the inner nirod it only has to be about 1/2" long, dont glue it in you will want to be able to change it as it will wear.Now just put it in your router and set your z depth just so the lead compresses the spring about 1/8 of an inch.I find this works very well because it keeps constant presser on the drawing surface,make sure you allow the correct z up for amount of spring travel.For the pencil leads you can either cut one out of a pencil or go to a stationary store and buy replacement leads.The hole assembly is only a few bucks and works very well.Happy drawing.
Greg Berscht

[ccr]

I'm using Enroute to create 3D lettering and as long as I set my depth deeper than the angle of the conic, the lettering comes out looking great. I am having problems doing the "fill" option in lettering and graphics. I can do hatch fill well enough, but when I try to island fill a letter such as "S," when the file is converted to the Shopbot software, it doesn't give me clean lines. Instead, it skips segments on the arc's where the z-axis is not changing and drills a series of seemingly random holes along the cut line. The same problems occur when I am engraving a large letter with a conic and I set the depth to a shallow distance (say -.1"). It gives me the typewriter effect. I have no idea what to do. I think I am outputting the file as dxf and perhaps I need to use g-code. I'm not sure what the difference is. I'm also not sure if I can convert g-code on my driver. If anyone can clear this up I'd appreciate it.

Cory Ryan
Artisan Goods
chorby@pioneerplanet.infi.net (mailto:chorby@pioneerplanet.infi.net)

[support@ShopBotTools.com]

Hi Cory,

Why don't you send a copy of a sample .dxf file with the problem to Gordon or me at ShopBot and we'll at least figure out if its a problem with the dxf conversion or with what is happen between Enroute and dxf. Try us at: support@ShopBotTools.com (mailto:support@ShopBotTools.com)

PS If your using recent beta software, also include the PROBLEM.LOG file from your ShopBot directory so we can duplicate your set-up. Thanks.

[gordon@shopbottools.com]

Corey,

I've had a similar problem using SignLab. They both seem to have a hard time handling narrow sections of letters. I haven't tried using the g-code output from Enroute, if you would like to try I can send you our g-code converter.

As Ted suggested, a sample DXF file would be helpful for us to ensure that you aren't having a converter problem.

[ccr]

Gordon~

I'd like to try the g-code converter, that is: if it is different from the converter found in 2b10. Maybe if I run it as an outboard program, it would have fewer glitches. Is it possible to convert the g-code, and then export it to an enroute readable format? If so you could convert your Enroute program and then go back and run it through again to check the lines. I'd like that. If you want to send me the converter, send it to cryan@infinitydirect.com (mailto:cryan@infinitydirect.com) Thanks a million.

Cory Ryan
Artisan Goods

[sheldon@dingwallguitars.com]

I'm trying to decide on weither to go with a second independant Z axis. One with a full sized router and one with a laminate trimmer for under 1/8" cutters.

When running two independant Z axis', does the second Z need to be zeroed every time it's used, or can the spindle offset be entered into software?

Thanks in advance.

[kenfox]

Sheldon,

Here is info received from Ted Hall on the 2nd
Z Axis topic. It is a little long, but the info is valuable.

If the bits are always in, then just physically determine the difference in location, by say drilling holes. But if the issue is that you'll be swapping bits around and are worried about height. Then you can use the ZZERO.SBP routine that is in the software in order to get an exact zero for for each axis. If you read the comments in that file, you'll get an idea for how it would work, I think.

In either case, once you know the values you will save these as variables in your files, and this lets you automatically and precisely switch between the 2 axes. The way this works is that after you change the default Z axis, you then offset its location using your recorded variables of the location. This may be a bit complicated the first time you program it, but you basically do the same thing each time. So, in your file, things would look something like the following:

' ...
' ... above here you have been cutting and are now ready to change Z and Acc
VI, , , , , , , 4, 3 'this line makes the switch
&NewX=%(1)+&AccX 'make var adding the offset to the AccX axis to current location
&NewY=%(2)+&AccY 'make var adding the offset to the AccX axis to current location
&NewX=%(3)+&AccZ 'make var adding the offset to the AccX axis to current location
VA, &NewX ,&NewY ,&NewZ 'this line Updates the Location
' ... now do some work using the new Z axis
' ... now when ready to switch back, just reverse process
VI, , , , , , , 3, 4 'this line makes the switch
&NewX=%(1)-&AccX 'make var adding the offset to the AccX axis to current location
&NewY=%(2)-&AccY 'make var adding the offset to the AccX axis to current location
&NewX=%(3)-&AccZ 'make var adding the offset to the AccX axis to current location
VA, &NewX ,&NewY ,&NewZ 'this line Updates the Location
' ... you're back where you started

These sections can just be put in your files to manage the two axes. Another option would be to set the 2 swap sections up in the Custom Cut section (try [C1] or look at [CS]) and this way the tools could be changed out with a couple of keystrokes from the keyboard.

Ken Fox

[annetts@mb.sympatico.ca]

Hello

I teach Technology Education in Mccreary Manitoba. We are thinking of using the shopbot with Mastercam version 8. Does anyone have any experience with Mastercam and Shopbot. I am especialy wondering if the converter will accurately convert all the toolpath information from Mastercam. Also how will it handle tool changes, offsets, etc. Any help would be appreciated.

Mike Annetts

[bwclark@centurytel.net]

Mike,

MasterCAM should work flawlessly with the ShopBot
G-code converter. If you do run into ANY kind of
problems, let me know.

As for tool changes, right now the ShopBot
software only supports a single tool. Now, the
G-code converter has a routine that will allow you
to change tools, but of course the tool has to be
changed manually.

Hope this helps. If you have any questions, feel
free to email me directly.

Bruce Clark
bwclark@centurytel.net (mailto:bwclark@centurytel.net)

[birdsofplay]

I believe that sb ( sbp files) can be run from
a script file that calls other sbp files.
You could set up each tool path and do a
return to 0,0 then change tool and rezero the Z
if necesary in between each tool path file.

i.e.

fp 1stcut.sbp
fp zeroz.sbp
fp 2ndcut.sbp
fp zeroz.sbp
etc
etc etc

I pain, fer sure, but a "way to get there "

[lakemar@accel.net]

Mike:

I have used Mastercam for programming my Shopbot for 2 years now. Bruce is right when he says that the converter runs flawlessly.
A few tips.
Write the toolpaths with cutter comp in computer on. Cutter comp in control should be off. You cannot comp for a different sized tool so the toolpath must be written for the size of tool that you will use.
Set feedrate and plunge rate the same in NC parameters so that only one feedrate is posted. After the file has been converted you can then easily set different feedrates. eg. ms,1,.5
Use the generic Fanuc post, mpfan.pst.
Set the misc. integer for part zero to 4. This will post G54 instead of a bunch of G92 lines.
Write your toolpaths as you normally would. Keep in mind that Shopbot does not support helical interpolation. If you wish to plunge in "Z" while cutting an arc the arc must be converted to lines because you can interpolate in all 3-axes.
After you have run the post there is a little editing to be done.
Remove everything from the safety block except "G90"
Remove "G54"
If you are using a relay to turn your router on keep "M03", however remove spindle speed.
Remove "G43" but keep the z-value in that line.
At the end of the program remove G28 etc.
Note: If you are using drill cycles remove G98 or G99 from that line.
If you can edit posts this all can be done so that the offending codes will not be posted. Most of them are in psof. G54=pwcs etc.
I have written a post for Mastercam 7.1 If you think it will work with 8 I could send it to you.
As for tool changes, I write different programs for different tools. At the end of the program I will change the tool, reset the height and run the next program.

Hope this helps
Dale