Plunging

[sascha]

We have our shopbot routing hundereds of holes, 20 mm deep each. The 2D files are originally drawn in Autocad 2000. I then save as DXF and open in Vector 8. I select the circles, copy them, and then paste them with a z variable of -20. Please note that the top of the cutting material is Zero. I then create the code and and convert to sbp format.

The tool will make two passes while running this file.

The first will plunge the Z axis to zero, and then run the file. So basically the first cut is an unintentional air cut. After completing the first pass, the tool will return to the starting point, plunge to -20 as I had specified during the copy comand. This pass will properly machine the lumber. This procedure is obviously a waste of time, and harder on the bit. Ideally, I would like to have 2 to 3 plunges through the material. I understand that I can adjust the plunge variable in the shopbot software(by editing file), but this is unrealistic when considering that we will need to route 1000's of holes when in full production, which leads to a very, very long code list. Is there a single variable that can be changed??What gives??

I have made sure that the coordinates in autocad are set so that the bottom left of the drawing is 0,0,0.

I thank you for your help.

Sascha

[odysseywood@home.com]

Sascha, In Vector8 once you have the circles selected move your cursor to the upper right side of the tool bar and right click. This should bring up a menu, select CAM tools. This should open a CAM Tool Bar. The sixth button from the left is your contour tool, selecting this will open a menu that will allow you to place the finished depth that you want to cut plus the depth for each pass. If you enter 20 for your depth and 5 for your step the machine will cut each circle in 4 passes. At the bottom of the contour menu is a check box for approach and depart, if you don't want an approach and depart contour added to your cut just uncheck this box and the machine will do a straight plunge. After filling in the contour menu click ok and then select insert NC from the CAM Tool Bar and then select generate NC. Hope this helps.

Sam

[Gerald D]

Hi Sascha, we also run AutoCad and Vector 8. Often we see strange effects with full circles and we have one foolproof fix; break a full circle into two half circles!!!

I know this sounds ridiculous, but we have given up trying to find out if it is a Vector or AutoCad problem.

[syp@earthlink.net]

Save your autocad dxf file to a acad release 12 dxf file. I have had problems saving and converting to shopbot files with other autocad version dxf files, but never when I save to acad rel. 12 dxf.

[donchandler]

I find that routing holes with a spiral down and a flat bottom pass is much better and you can cut faster. (use the shopbot routine) I draw the holes using points in Acad. this gives me a point at the center of the circle. I save as R12 DXF and load into vector.I move the axis 1/2" below the surface. I select all of the points. I wrote a macro that askes for hole dia. , bit size, how many passes and depth per pass. I load this into the sbp program, this lets me adjust hole dia, change to a different size cutter without changing the hole dia, allow for different thickness of part, etc. I then set vector to program the position of each point (J3,-2,-1,.5), followed by a line which calls a subroutine (GOSUB HOLE). At the end of the file I load the subroutine which is a CP command with (&) variables for all of the inputs.I also put a counter that displays the number of the hole it is cutting. This way, if I have to stop I know where it is in the list of holes, then I can use the FG command to start at the next hole. This idea can be used for square holes also. We do lots of parts with 800-1000 holes each and in a pattern that does not allow a array program, such as the example in the SB software, to work. I can produce a complete program this way in 10-15 min. and it will cut better than the straight down plunge.

[sascha]

Thanks to all of you for your help. Great forum!!

I succesfully routed some holes, in two steps, plunging 10mm each using the contour routine, with the approach/departure option turned off.

I would like to spiral cut the holes next, so I will look into writing a macro.

Again, thank you all for your quick and intuitive responses.
Sascha

[gdorrington@iafrica.com]

Hi again Sascha, I see on your website that you have German connections (apprenticeship in München), are you any relative of the Ott's of Mainz? (Harald, working in Laubenheim).

[davenadeau]

Sascha,

Regarding spiral cutting of circles in Vector, it's easy to do by adding extra parameters to the CG circles written by Vector. This can be made even easier by making a simple macro in Vector to automate the process. Here's how... After you generate code in the NC window in Vector, move your cursor to the CG lines for the circles to be cut with a spiral plunge. Note that not all CG commands in the NC window will be for circles since Vector also uses CG commands to describe arcs in any rounded portion of a toolpath (you can watch the red arrow in the drawing window to tell you when you are on the correct code lines for your circles). Put your cursor at the end of the CG line (the line will end with a 1 or -1 depending on cut direction) to add parameters to specify how to do the spiral plunge. Assuming a normal set up in which Z=0 at surface of material, I add the following to the end of CG lines for circles I want to spiral cut:
,-0.1,5,,,4,,1
The commas are used in standard ShopBot fashion. The first comma would be placed immediately after the 1 (or -1) direction parameter as a separator comma, and the commas immediately following each number are separator commas also. The other commas are "placeholder" commas to skip parameters that I don't want to change. The -0.1 in this example is the depth-per-pass parameter, and the 5 in this example is the number-of-passes parameter. The 4 in this example requests a "spiral plunge with bottom pass" although I could have substituted a 3 for a regular spiral plunge (theoretically you can also substitute a 2 here for pocketing within the circle, but I haven't tried it). The final 1 in this example requests that plunge depths be offset from zero (as is the case if you set Z=0 to the surface of your material). Thus, this example codes for spiral plunging with a bottom pass to a total depth of -0.5 inches.

Of course you can always manually type these parameters into your code in Vector, but you can simplify the process of adding these parameters by using the Windows clipboard or Vector macros. You can try the Windows clipboard by cutting the text above from this message and pasting it into NC code in Vector. If you want to change the depth per pass and number of passes, then you can simply make the change once, copy to the clipboard, then paste the modified text into the code for the remaining circles. Vector macros make this process even easier... In Vector you can create a macro from the NC window using the Options,Macro command. Copy my sample code above to the clipboard, then in the Options,Macro window type the name of your new macro in the Menu Text box and click Change. This sets the name that will appear in the Macro menu (I call my macro "Spiral Plunge"). Your macro name will eventually appear in the Menu List of the Option,Macro window under the name you select, but it is still a blank macro at this point. Click the "Edit" button in the window to add lines of text to your blank macro. Type your sample parameter code in the "Edit NC Lines" window or, if you have copied my sample code to the clipboard, you can use CTRL-V to quickly paste the code from the clipboard (CTRL-V is a Windows shortcut for Paste). Click OK twice and your macro can be inserted automatically by selecting the macro name from the Macro menu.

It's nice to know that even though you use Vector to toolpath a circle you don't have to sacrifice the ability to spiral plunge. Using a macro makes spiral plunges quick and easy in Vector. Give it a try.

Note that if you are not familiar with the parameters specified in ShopBot circle commands, you can use the HC command in ShopBot to bring up a command help page. Go to the CG command to get a list of all parameters (in the correct order) with a detailed explanation of how each parameter is used. In fact, if you look up the parameters for the ShopBot CG command (G-Code Circle) you will see that the parameters at the end are the same as those for the CC (Cut Circle) and CP (Cut Circle Around a Point) commands.

Regarding your original post, I'll venture to guess as to why your file cut circles at 0 and -20.... You said that you copied and pasted your circles in Vector. When you displaced the copied circles to -20 mm depth, you then would have had two circles at each location (one circle at depth 0 and one circle at depth -20). If you still had the original (depth 0) circles selected when you generated ShopBot code, then circles would have been cut at both 0 and -20.

Apologies for the length of this post
Dave

David Nadeau
ShopBot Tools
Technical Support

[dmdraper]

Dave, don’t apologize - that was all great info!

Regarding macros in Vector, I have created several using the method you described and they show up on the list in the Macro menu in the NC window until I close the drawing (using update/save), then the macro is gone, i.e., the next time I start a new drawing or even open the same drawing, the macro is not in the drop down list. There must be a way to save the macros you create for future use because the Start, End and Version macros are always there, but I haven’t figured out how. Any Ideas?

Dave D.

[jkforney@yahoo.com]

Dave D
You have to change the attribute on one of the files from read only. I think it may be the ini file but I could be mistaken. I'll check later when I have more time, just got back from the Woodworking show in Anaheim and a long vacation.

John Forney

[dmdraper]

Problem resolved.... the file that needs to changed (i.e., remove read-only attribute) is the ShopBot driver for Vector - in this case, shopbt2f.cfg. Thanks for the hint John.

[toys]

I've been testing out Vector and can't figure out how to plunge straight down and straight up.

In Turbo Cad I used a single point. Vector seems to automatically delete single point line segments.

[toys]

I figured out the following. If I press P I can move the origin to where-ever I need a plunging line and then use the coordinates line drawing function to draw a line straight down.

Is there any special function to make a plunge and pull up slightly and then go down some more?
A sort of pecking. I thought this might be easier on the router bearings.

My cutter is 1/4 " and I want my hole to be 1/4.

[gerald_d]

David, in my Vector 9.4 I have Draw > Point that (ahem) draws points. When I select those points and do a Draw > Other Curves > Connect at Z, the tool just does a single plunge at those points as you would expect and want.

My Vector imports points from AutoCad flawlessly.

A jerky plunge is something that you would have to program manually - but I don't think it will do much for the router bearings. Have you put a router bit in a drill press to feel how easily/difficult it drills? IMHO 1/4" bits drill fine - it is the bigger bits that don't like vertical plunging.

PS. Ron Brown will post 1 minute after me.
Here's Ron........

[rgbrown@itexas.net]

"Vector seems to automatically delete single point line segments."

My GAWD.... all those cribbage boards I made don't have any holes in them...... They LOOK like they have holes but the holes must be virtual.

Actually David what I do is draw cribbage boards in one of my CAD programs - or sometimes Vector and put points at the depth I want the holes. The connect at "Z" command gives the up and down movements.

[toys]

Thank you for the info. Would you like to have a virtual leveling of ... your parts files? I'll let you have it (the program) if you like
Are you guys for "real", on vacation together or cell phone buddies?

[toys]

Hey Gerald_D Brown,
Do yawl have use parts wizard? And if so are there less steps to go from a dxf file to a sbp file? I'm trying to figure out what program I want to get for generating tool paths. Have you tried the STL program Fred smith sells?

[rgbrown@itexas.net]

David,

The least steps is the FC command in ShopBot. I am to early of a user to have Parts Wizzard. Now that I have a fundemental understanding of Vector, I see little need of anything else.

I am also one not to experiment with multiple programs. Once I find a program that works for me, I stick with it. I only upgrade when I feel the upgrade will benefit me.

I used the F_ile C_onvert in ShopBot to show a person this week that, "It can be done." It has been two or more years since I used that command.

I still don't use but about 30% or less of the ShopBot commands. Each person will have lightly different needs and uses for a CNC machine. IMO, if anyone tells you, "It has to be done this way." probably needs to have a diaper changed and probably for the same reason you change a baby's diaper.

I think one could use a program like RHINO, that allows line offsets, trimming and joining to build cutting files that work. These would be exported to ShopBot and the UC/FC command would convert them to "Code". I draw bit approaches in RHINO if I have a need for that feature. I also build "hogging files" in RHINO. I do export them to VECTOR to assure the proper order.

[toys]

Virtual Ron or Gerald,
There are a lot of cutting techniques that are difficult to do using UX (FC for you new guys). I've found that approaches and cutting direction are very important if you want a good cut. It's a pain using just CAD and no CAM function. If you don't do things a certain "way" you end up with the "dirty diaper" in the form of lots of sanding and filling and ... sCrap.
Has anyone used Vectors Macro Tool Bar to speed up some wood working techniques like lead ins and outs, multiple passes from oposite directions for rough passes and finishing passes. These things do make a big difference and would be easier if there were short cuts available. Would it be easier to use something like DeskCam or Parts wizzard? I'd like to hear some real "non-virtual" people talking about real problems (wood- related) that need real answers(sometimes with software).

[gerald_d]

David, and all the other suspicious readers, I am not Ron!



I editted my post after I saw that Ron had posted. Have you guys noticed the Edit button after the time stamp on each post? Apologies to Ron and David for being the victims of my joke.

Thanks for the offer of your "virtual leveller" - I have no need for it today, but when I do, I'll call you for the latest update of it.

I have found Vector to be pretty darn fast and accurate to go from dxf to sbp. I didn't think so at the beginning because of the long learning curve (of which I havn't seen the end yet) but it has really paid off now to stick with one product and learn it "good".

Having said that, we use AutoCAD to make the dxf, and it is during that process that we plan the cutting. The lead ins, etc, we draw in AutoCAD, before going to Vector.

[rgbrown@itexas.net]

Well David,

You have asked about a program I don't use. I do know one can get order and direction in Vector. I feel other programs will allow one order and direction. Vector has a forum. I believe they discuss pecking cycles and macros there.

My point on certain ways was about software and CAM programs but, you seem to have a "way" figured out, I doubt you need any help I might offer.

[toys]

Vector is incredible!!!! Wonderful!!!! And does beautiful lead-ins and outs. There Macro program MTB is very easy to learn compared with programing in Basic. You can easily automate various ways of doing pockets, offsets, . . .
Two AM that is when your brain shuts down enough to get out of the way of learning new exciting things. Yehaaa, Thanks Fred Smith for Vector support, Ted Hall and the ShopBot Gang for your support. You all deserve a round of aplause.....clap clap clap

Thanks for the info Bob and Larry I mean (Ron & Gerald) I think I'll call you the virtual twins. You don't want to help but you just can't stop yourself from helping anyway or at least ribbing everyone. The "SB Virtual Twins" Touche'
It would be nice if we had those animated feally buttons as the Vector forum has. LOL I gota go to bed. Good Night ShopBot! :0

[gerald_d]

Good night David.
4449

[toys]

And a late Good Morning to you. Cool graphic, too bad its not a point and click away, like Vector Cad/Cams. Hey, where did you get that one its not in the forum list?

[gerald_d]

You say that I don't want to help
4450 , so I am not
4451 going to tell you!
4452

[toys]

It took a while but I figured it out just like Vector Cad/Cam.
4453

[gerald_d]