Newbie- Need help with profiling function with bobcad

[jodybo]

Hello,
I am using bobcad, and when I choose to do a profile, the only way I can get the part to come out is to use offset right, when i generate the code it always conventional mills, I need to climb mill and use g41 (left) but when I do it does the profile inside of the lines of the object I am cutting.
thanks for any help

[BurrMan]

You can create a "contour" from your geometry and control direction with this.

[zachf]

Burrman,

Can you explain this in more detail. I can't seem to figure out how to climb cut.

Zachf

[BurrMan]

When you create a contour, it has little arrows on it. The profile will cut in the direction of the contour. There is a command to reverse contour. to change the directions. I was suggesting controling the direction with this. But I didnt try to setup a file with all the G41's and such and test it. If you have a sample file we could be sure we are talking about the same thing.

[zachf]

Burrman,

In V23 I don't have any arrows depicting direction unless I am selecting for an offset function or something similar. When selecting geometry in the cam tree there is no directions on the lines to be selected. I did find the reverse contour function and I tried it, but there was no change in the cut direction when I verified it.

Zach

[lynn mynatt]

Very GOOD!! I've been trying to figure this out as well. Zach, the contour is located in the "other" menu. Click contour, select your preferences then select your profile. You will then have to edit your your feature settings under cam tree for that profile. You will want to select g41 or cutter left. G41 didn't work for me but cutter left did.

Burrman, can you explain what the difference between G41 and cutter left is and why both are here?

[mcphill]

Note, to select the whole chain to make it in to a contour (like the four sides of a box, for instance), hold the shift key (I think, it may be ctrl) and click on ONE piece of geometry. All the connected pieces will be highlighted. Right click, then click OK. If your source geometry is not all connected (overlapping line segments, or opens in the segments) you won't get a good contour. Use the trim and extend commands to make all the lines connect perfectly before creating the contour.

[zachf]

Thanks,

I got it figured out, but what a pain in the ***. They really need an option in the feature for you to just click if you want to climb cut. I am going to put a request into their forum for this for any future updates. Thanks again for the replies.

Zach

[BurrMan]

Originally Posted by lynn mynatt Burrman, can you explain what the difference between G41 and cutter left is and why both are here?

Well I'm not the best machinest but I think it is this:

Cutter left/right actually calculates the toolpath to that side. G41/42 just inserts that G Command into the code and the "Machine" does the offsetting. When why and how to choose one or the other would be beyond me. I think it just has to do with your particular setup and having the options. For instance, with our simple setup, we choose to have the toolpath offset to keep it simple and not try to make our machine do the work.

G41 didn't work for me but cutter left did.

To get your G41/42's to output you need to choose a "lead in/out" other than vertical.

[BurrMan]

Just a side note with regards to creating Contours. It actually makes a "New entity" as the contour. so if you select a ceated contour and delete it, the underlying entity geometry is still there and you can re-create a new contour.

[BurrMan]

Originally Posted by zachf Thanks, I got it figured out, but what a pain in the ***. They really need an option in the feature for you to just click if you want to climb cut. I am going to put a request into their forum for this for any future updates. Thanks again for the replies. Zach

Hi Zach, I have seen this come up before. It may be that having a "Contour that can control direction" is much more flexible and powerful and then having a choice in the feature could create conflicts and confusion.

There may be another answer coming also as I have have seen direction be controled in other ways depending on the feature operation and methods.

[mmc005]

Burr is correct in how the offset/Gcode works. You just have to remember to put your tool radius into your tool offset page before you run the program, otherwise the machine will not pick up the offset and will cut your part wrong.

As far as why to choose a direction for cutting, there are many reasons this. Back in the day of manual machining you had backlash(thread wear) in your lead screw, and could only conventional mill with any feed stability. If you tried to climb mill, it would pull the table into the cutter because of the backlash. With conventional milling the cutting forces oppose each other and cancle each other out(no table pull). With CNCs or automatic feed machines, this is not an issue. Climb milling typically gives a better finish than conventional milling and your setup can dictate which you have to use for cutting forces vs. work holding.

When your picking your 2d profile, just choose the lines in the order and from the direction that you want the tool to cut, this will eliminate any confusion on which way the offset will be.

Dave