[winaa]

How do I do a cut-chain in version 21 or 23 I have read about it on here but can't find anyway of doing it in the software. I have drawn some tool paths that I want to cut.

[BurrMan]

Hi winaa,
A chain refers to a "continuous selection" and sometimes requires a "shift clcik" to create it..

If you create a default ellipses in V23, note that it is made up of several segments... If you shift clcik one entity, you will see the entire thing highlight.. This means it is one continuous chain selected... You can select that as geometry for your cuts..

There is also another thing about chain selecting and that is it can determine the "direction" of the selected enteties. To see this, you can create a "contour" out of the default ellipses. If you go to the other menu and select contour, then go to your default ellipses and shift clcik it. You will see an arrow indicater.. Notice that the arrow can change depending on which side of the initial segment you clcik on. Now single clcik an entity of the ellipses while in the contour command. You can single (No shift key) clcik the entity at either end to change the arrow direction. Then continue single clciking in the direction of the arrow about half way around. Then you can shift clcik an entity half way to end the selection.

Does that make sense?

[BurrMan]

Here's a couple videos:

YouTube - ‪chain selection‬‏

YouTube - ‪chains2‬‏

[winaa]

Hi Burrman that sort of helps but what I am looking for is as follows


#1: Get 2D geometry of the part I'm attempting to make. This is either done in Autocad from scratch or is imported into AutoCAD from either Inventor or Solidworks.

#2: Determine the profile(s) to be machined and isolate it from the rest of the geomery ( usually copy the geo )

#3: Use the tools in AutoCAD to draw a circle to indicate the work 0 position and draw geometry ( lines and arcs or whatever ) to represent EXACTLY what the toolpaths I'd want. That is offset lines, trim them etc etc, which will result in a single chain of geometry that is representative of the exact center of the toolpath which I'd what the cutter to follow.

#4: Take the resulted geometry ( and only the resulted geometry) and export it as DXF. Note that this may be multiple copies of similar geo, each resides as a separate set of geometry of the EXACT toolpath I'd want with a circle indicating the work 0 point.

#5: Import the DXF into Bobcad ( currently). Move BobCAD's X/Y/Z0 indicator to the center of one of the circles ( the work0 location of that particular toolpath), and then create a cut-chain. This cut-chain op does not create any Z movements, does not enter any feedrates, does not attempt to create a canned cycle, does not do a darn thing other than takes the geometry and enters text lines starting with the appropriate G01, G02 or G03. That is it and that is all I want it to do. No logic, no computation, nothing. Just type in the endpoint of the entity and add the appropriate G-code in the beginning and add the I and K value at the end ( in case of arc movements )

Reason for this is that we have some well proven tool paths drawn up at work that we used on our older machines now we have brought a new machine and bobcad-cam I would like to use these paths but in a more automated way.
The above steps are copied from another thread I have read and the cut-chain/Auto Route sounds exactly what I am looking for but I can't seem to find out how to do it.

[dougl]

Hi Winna,

Have you tried using the 2D engrave toolpath? If I am understanding what you are trying to do and you are drawing the actual toolpath I think this would be your tool of choice.
As far as moving the zero point coordinate in Bobcad V23 you will have to translate the part to the zero.

Something to play with anyway.

Doug

[BurrMan]

I'm not sure I follow well. But going off of what dougl said, the "0" can be changed for 2d cuts by setting the UCS. Snap a UCS to the center of an arc and make it active. The code should post as 0 from there..

V21 has a function that creates geometry from G-code, so if you have previous toolpaths you want to use, V21 should do that, but I dont know V21.

Maybe someone else knows what you are asking for?

[winaa]

Sorry that last post of mine was not very clear, basically just step #5 in my posting(just convert the lines and arc's to G01.... G03.... etc)
The 2D engrave toolpath sound's like it will do what I want. I have attached a .dxf of an old tool path. basically I want to start at the start point using a 50mm side and face cutter and follow the arc's and lines to the circle then follow the circle round and exit on the last arc.
I know this is a simple tool path but its the only one i have at home the rest are at work. I suppose what I am trying to do is a bit of a cop out on not learning bobcad-cam properly. What I will do (when I get back to work) is post a drawing of the part I wish machine in a new thread and go from there.

Burrman our old machines have Heidenhain controllers that are programed in their plan data entry language not G-code.

[BurrMan]

Hi winna,
Here is a BobCad file to depict what you need to do to the geometry. (I think this geometry needs to be scaled down by mm???)

What you need to do is break the circle at the point of entry, so you can direct the contour into the arc to go around it before the exit arc..

After you get that break there, you can create a contour by picking the chain from start to finish, then it will turn into a contour entity with direction, as in this file.. I just toolpathed it with a profile-no offset.. I included the default output code from my post, that predator editer can backplot to show you the cut...



The code output by this is formatted by your "post processor"..I think there are heidenhein posts for BobCad.. This will determine (And can be configurable) to output the toolpath code however your machine needs to read it.. Do you have a Heidenhein post loaded for your BobCad already? If you do, post this file with it and see if it formats as you want.. If either not, we can talk more about this.

I dont understand the heidenhein type output, Maybe someone else already has something for you.. I could help, but it may be more painful for you just because I dont really understand what the expected output should be like..

[BurrMan]

For instance, here's that same file output with the heidenhein 2500 iso post from the BobCad website linked to here:

%100 G70
N1 (P000-1236.NC)
N2 ( HEIDENHAIN  2500)
N3 (SAT. 07/09/2011 01:20PM)
N4 G01 G40 G90 X+0 Y+0 Z+1 F999 M00
N5 T0 G17
N6 G00 G40 G90 M06
N7 G99 T1 L+5. R+.25
N8 T01 G17 S374
N9 M03
N10 M08
N11 G00 X+0. Y-104.996
N12 Z+.1
N13 G01 Z-.5 F+.9
N14 G01 Y-94.996 F+1.5
N15 G17 G02 X-8.2017 Y+94.6413 I+0. J+0.
N16 G01 X-84.6153 Y+103.5553
N17 G17 G03 X-99.773 Y-88.7027 I+1.7773 J+.0176
N18 G01 X-164.99 Y-101.53
N19 G17 G03 X-199.99 Y-66.53 I-199.99 J-101.53
N20 G17 G02 X-199.99 Y-66.53 I-199.99 J-1.53
N21 G17 G03 X-234.99 Y-101.53 I-199.99 J-101.53
N22 G00 Z+.1
N23 M09
N24 M05
N25 %100 G70

Heidenhein Posts

The output changes dramatically depending on the post used... When we get that straight, it should do what you need.

[winaa]

Hi winna,
Here is a BobCad file to depict what you need to do to the geometry. (I think this geometry needs to be scaled down by mm???)

What you need to do is break the circle at the point of entry, so you can direct the contour into the arc to go around it before the exit arc..

After you get that break there, you can create a contour by picking the chain from start to finish, then it will turn into a contour entity with direction, as in this file.. I just toolpathed it with a profile-no offset.. I included the default output code from my post, that predator editer can backplot to show you the cut...



The code output by this is formatted by your "post processor"..I think there are heidenhein posts for BobCad.. This will determine (And can be configurable) to output the toolpath code however your machine needs to read it.. Do you have a Heidenhein post loaded for your BobCad already? If you do, post this file with it and see if it formats as you want.. If either not, we can talk more about this.

I dont understand the heidenhein type output, Maybe someone else already has something for you.. I could help, but it may be more painful for you just because I dont really understand what the expected output should be like..

So you added the break to the circle then picked the chain getting the direction correct and used 'contour cut' with no offset to create the G-code?
Sounds exactly what I want to do.

[BurrMan]

So you added the break to the circle then picked the chain getting the direction correct and used 'contour cut' with no offset to create the G-code?
Sounds exactly what I want to do.

Not exactly. I broke the circle, then I ran the "contour command" from the "other menu", then I selected the chain as I wanted it to cut and chose "OK". This creates a "contour" which is a continuous chain with direction... Then I selected the 2d operation "Profile" and selected the newly created contour as geometry and computed toolpath...

The code output will be formated by the "post processor" you choose from within the Cam tree, to create the toolpath at the machine level..

I need to make a short video for another thread here, I'll try to include making one of this short process too..

[winaa]

thanks now i am on the right track I should be fine.
I will still post one of our jobs to get a different view on machining the part.
We are still in the mind set of making as simple tool path as possible after doing years of manual coding. Now we have CAM we should be thinking about efficient machining and not simple tool paths.
Aaron

[BurrMan]

In the profile dialogue, you can explore the leadins/outs. They will have "radius" and parallel and such, to create those that you have drawn there in your part..