Help!!!!!!

[margate_stair]

I'm New to all this & have some background in CAD my question is very simple I guess
Say I wanted to crosscut a 5/4x 12"x6' pc of lumber, why can't I just draw a straight line & have the SB cut it, why do I have to double the lines & close the ends to make this cut

[beacon14]

You can do what you want by choosing the "Machine along Vector" toolpath in PartWizard or "Profile" with "on" selected in VCarve Pro.

[margate_stair]

Im working in Part Works when I draw the line it only calculates a tool path when i use the machine on, not outside or inside does that mean I have to make deductions for bit size

[richards]

Gregory,

Let's work through this with PartWizard. (I have version 2, so your copy might be different.) Here are the steps that I would take to crosscut:

1. Create a new setup X = 72", Y=14", Z=1.25" (The Y-size is larger than needed to allow a total crosscut.)

2. Click the Create Polyline Icon

3. Enter Next Point X to equal the center of the cut on the X-axis.

4. Enter Next Point Y as 0

5. Click Add

6. Enter Next Point Y as 14

7. Click Add

8. Click Close

You now have a single line that is crosscutting the lumber.

9. Click on Toolpaths

10. Click on Machine Along Vectors

11. Select tools, depth of cut, etc.

12. Select the line you wish to cut.

13. Give it a name, i.e., x_cut_1

14. Click Calculate Now

There you have it, a single line that can be used for crosscutting.

Remember that the Y-size was specified as being larger than it really is. That was done to allow the cutter to pass completely through the lumber, side to side. Because of that, be sure to position (clamp, etc.) the piece of lumber about 1-inch from the edge of the table, taking care to have everything parallel to the edge. Then, when the cut is made, the Z-axis will plunge to whatever depth you have specified and crosscut the piece of lumber.

Once you've done this a few times, you might want to just write your own file, using your favorite editor. If you decide to do that, and if you need some help, just post your question on the forum or email me directly (click on my profile to get my email address).

[margate_stair]

Mike
Thanks for the response, I think one problem is SB E-mailed me partworks I guess as part of the new software package (machine comes in two weeks)& there is no machine on vectors command it just gives me a Outsde,inside & on command, when I hit the outside or the inside command error comes up open vectors

[richards]

Gregory,
I was wondering about Partworks software. It's a program that I've never heard of.

Here's a sample of a simple file for crosscutting, using four passes to get to depth. It is assumed that the piece of lumber is 12" wide and 72" long. It is also assumed that the piece of lumber is located at the 0.0, 1.0 point on the table so that there is one-inch between the edge of the lumber and the edge of the table. The sample shows two crosscuts, one with the center of the cut at 12" and one with the center of the cut at 36"

SA
' First cut, centered at X=12
JZ, 2.00
J2, 12.0, 0.0
MZ, -0.3.125
MY, 14.0
MZ, -0.625
MY, 0.0
MZ, -0.9375
MY, 14.0
MZ, -1.2575
MY, 0.0
JZ, 2.00

' Second cut, centered at X=36
J2, 36.0, 0.0
MZ, -0.3.125
MY, 14.0
MZ, -0.625
MY, 0.0
MZ, -0.9375
MY, 14.0
MZ, -1.2575
MY, 0.0
JZ, 2.0
J2, 0,0

END


You could dress up the program by using INPUT statements to find the coordinates of each cut, depth to cut per pass, etc. In any case, you'll find that straight cuts along vector are very simple to make.

[ryan_slaback]

Gregory,
A single line is just that a single line. You can not draw on the outside or inside of a line. You can however draw on a line. In order to machine inside or outside you need to have a closed shape like a box, something 2d. A line is 1 dimensional.

[margate_stair]

Thanks to both you guys, I was using a straight line as a example, we are a stair builders & I thought that a SB would be more versatile than a stair router, so are cuts are mostly going to be stringers,both housed & open,treads & risers & hopefully down the road Railing parts.
If any body else would chime in I would appreciate it.

[kirkkelsey]

What CAD package are you using to create your parts? Are you trying to create your parts in VCarve Pro or the Part Wizard?

I would recommend using a 3D solid modeling package to design your stairs and parts, output DXF files of your stair parts, and code them in VCarve Pro.

[margate_stair]

Using AutoDesk, I haven't used parts wizard yet they sent me Part Works, It seems easier to create in AutoDesk, What do you think

[fleinbach]

David,

This Shopbot has a Columbo 3HP spindle and has had very little use. They picked it up from a leasing company.

[richards]

Gregory,
There seems to be a lot of different AutoDesk products. I use AutoCAD LT for most of my design work. After designing the parts in AutoCAD LT, I save them as DXF files and then use PartWizard 2 to create the tool path file. That has been working well for me since I got my Shopbot in July of 2004.

[garyb]

Per Shopbots announcement Parts Works is Shopbots version of vcarve pro which is now shipping with all machines

[kirkkelsey]

I have not used PartWorks/VCarvePro for design (http://www.shopbottools.com/software_v.htm), but think it is easier to create designs in a CAD tool such as AutoCAD than most mixed CAD/CAM software. While 2D CAD is fine to create simple part outlines, it is lacking when creating multiple parts that fit together because the design relies on the users skill in making sure the parts fit. We migrated to 3D solid modeling and feel it is a far better choice. However, once you determine what design/CAM combination will accomplish what you want to do, then be prepared for some experimentation and sample projects to learn how to use the tools.

I agree that a ShopBot is more versatile than a stair router, then again it will take more effort to learn to use a multiple purpose tool than one specialized for a particular task. However, the most valuable thing about owning a ShopBot is THIS user forum, and the people that always seem willing to help one another.

[richards]

Okay, now that I know what Parts Works is, I've found that you can create crosscut tool paths with that program (VCarve Pro). It actually takes a little longer than it would to do the same thing in PartWizard or AutoCAD LT, but it can be done. (On the other hand, VCarve Pro excels at doing more complex things.)

Click on Draw Polyline

Draw a single line while watching the X/Y coordinates at the bottom of the screen

Press Esc when you have the line drawn

Click Node Editing and adjust the endpoints (if necessary)

Click Switch to tool paths tab

Click Create Profile Toolpath

Enter the cut depth, select the proper tool and click Machine Vectors On

Enter a name for that toolpath

Click Calculate

Click Save Toolpath

That's basically all that there is to it. You can do much more, of course, that that will get you started.

[randy]

Here is how I make a simple cutoff using VCarvePro:

Material size = 1.5" x 11.5" x 96"
Bit size = 0.50"
Desired length = 40"

1. Create material using lower-left corner as XY origin position and no offset.

2. Create a rectangle (box)that is slightly wider than the bit and tall enough to cut through the width of the material. In this case, 0.501" x 14". Offset the rectangle for the length of the desired piece and slightly outside the piece. X = 40" Y = -1"

3. Create a pocket toolpath that will cut through the material.

Three steps and you are done.

The reason for adding the extra 0.001" is that VCP will not create a pocket that is exactly the same size as the tool.

[margate_stair]

Kirk is right on with the response from you guys Thank You
Mike I see what your saying but I would have alter the sixe of my cut to allow for the bit size.
I was kind of thinking what Randy said but using the offset tool instead