What is the proper way to program a counter bore using an end mill in V21? Everything I've tried so far just does a Rapid to the bottom and then does a spiral. My Anilam uses a Circular Pocket to do this.

John

It seems as if you are only picking point and performing a final cut without any roughing type operations.
I would make a circle. Create the spiral path for the endmill. When you pick the spiral set the correct depth and perform roughing. If you did not make the circle smaller (for a finishing cut) the diameter of the circle will be already at size but the depth will be the only 'finishing' routine.

It sounds like you are cutting to final depth to start with. If you are trying to use a specific call routine your Anilam reads then you are on your own.
I also have no idea as to your ratio of endmill to counterbore size or if you have counterbore within counterbore.
From what I read I believe you problem is from lack of roughing depth being set.

mc_n_g

Where do I set the correct depth?

John

There are several ways to c-bore.

Try this.
1) draw circle at part top.
2) select circle and go to menu 'Other>Pocket>Spiral
3) Now set all the parameters includiong 'mark start' and if you intend to finish afterwards then click OK.
4) On NC side select the 'Tool Depth Settings' (up/down). Set the settings there including turning on the roughing if needed. This is where the depth is also set.
5) Selct path generated on the cad side if not alread selected. The entire path can be selected if you view in isometric and hold the shift key while clicking near the start line top.
6) On the NC side select the 'cut all'.

There are other ways to do this too.

Where is the Tool Depth Settings? In help it shows the Machine menu when you select the tool depth settings but there is no Up/Down in there...

John

Where is the Tool Depth Settings? In help it shows the Machine menu when you select the tool depth settings but there is no Up/Down in there...

John

John,

The Up/Down Button is on the CAM Side of the Software.:) See Pic at bottom.

It looks like this:

u....
d....

I tore the menu up looking for that and it's a button on the side bar.

Not the most windows compliant software I've had the pleasure of using...

Thanks Again for your help
John

YW John,

How is it working for you now?

One thing you can do as well is add the settings to a macro call. The macro can then be added to the menu. So you can set all the variables using your own window, instructions, wording, and have it tied to lets say --the auto run feature.

Just some of the things Bobcad can do. But even if there a few things you may not like many of them can be modified to meet your needs.

Toby it's getting better...

tjones, I'll look again at the macros. I have a v18 and 19 manual to look at as well as the v21 downloaded manual.

Got to program a little PLC then I'm back on BobCad like a chicken on a june bug...


Thanks again for the help
John

I made this one today between runs. Juts add it to your windows menus and you can set a keyboard shortcut to it. You can also link it to other functions. For instance have it run prior to your pocketing.

These are a few ways to use scripts in Bobcad.

tjones, That is cool. I had to make a mod to it to get the output format correct.

Before = Arc Cw X1. Y0. Radius 0.5F1.5
After = Arc Cw X1. Y0. Radius 0.5 Feed1.5

Now I need to study it a bit to see how I can make it do a G77 output

CircPoc Xn Yn Hn Zn Dn An Bn In Sn Kn Pn

Where
Xn = XCenter
Yn = YCenter
Hn = StartHgt
Zn = ZDepth
Dn = Diameter
An = Stepover
Bn = DepthCut
In = RoughFeed
Sn = FinStock
Kn = FinFeed
Pn = ?
etc.

Is my thinking correct that with the correct macro I can pick a point on the drawing and select CircPock and fill in some blanks and it will generate the G-Code?


John

Is my thinking correct that with the correct macro I can pick a point on the drawing and select CircPock and fill in some blanks and it will generate the G-Code?

John


No and Yes. As far as I know the user scripts will not allow for screen selection during execution. So you would need to work around it.
Here are a few ways.


First there is the easy way. Bobcad will modify a post for features like this to be added (free). They are very good and have a simple form to fill out.

Second. Know the coordinates and enter them manually.

Third. Do an extra step. (I like this one) Click the point and in your script have it run the 'Move to Point' feature. You will get 2 lines of code in the NC window but use the script to read the code for the X,Y position. And then change those lines to what you want them to be (your G77 code)

The third way just uses the built in features and the NC window as a temp to hold the coordinates to use in the script.

Try recording scripts to get ideals of several functions and open the available scripts to get more info.

The Askheader makes the simple input window and there are many other undocumented features people list a little of everywhere.

I have pasted several of the ones I think are usefull in a small file and Bobcad tech has list one doc that has some good definitions as well.

Here is a g13 hole milling script that you may find useful.

(don't know who wrote it)

G13 milling script would be best placed in the Cycles menu. This would allow you to select more than one point and esecute the same commands for each selected point. Plus, you don't have to input the point coordinates.

Basically it's like this:

Using the Setup -> Cycle option, add a new cycle called whatever you want and add it to the list. Then Click on the Modify button and input @c in each of the fields. Make sure you hit ENTER after you input the @c, otherwise all the coordinates end up on one line. Then OK out of modify and put the name of your script in the Script box. Next create the Script. Following is a basic example of how it 'could' be handled.



'set up your variables

'ask the user for input

NCEdit Output, Line = i 'this tells us what line we are starting on and assigns it to a variable

Generate 'this outputs the coordinates of the selected point(s)

'then do your code modification using a loop for any number of points



Regards

G13 milling script would be best placed in the Cycles menu. This would allow you to select more than one point and esecute the same commands for each selected point. Plus, you don't have to input the point coordinates.

Basically it's like this:

Using the Setup -> Cycle option, add a new cycle called whatever you want and add it to the list. Then Click on the Modify button and input @c in each of the fields. Make sure you hit ENTER after you input the @c, otherwise all the coordinates end up on one line. Then OK out of modify and put the name of your script in the Script box. Next create the Script. Following is a basic example of how it 'could' be handled.


Regards



So if I understand correctly then this will allow you to select a point during execution of the script?