[blowncoupe]

I just got V27 pro and my 3d tool paths don't go all the way to the bottom of the part .I have tried z rough, z finish , planer they
all leave about .250 from bottom . Z 0 is the bottom Z+1.00 is the top . I have even moved the bottom of part up .500 and still
the tool path didn,t go down all the way about .250 from bottom. Are there defalts from keeping this from working? I have V23
and the tool path works just fine but it doesn,t have 3d machining I only have mill 1 in it

thanks

[jrmach]

Can you .zip a .bbcd file that we can look at ?

[blowncoupe]

I sure can . what address do I send it to?

[mmoe]

Post it on the forums here using the "Go Advanced" button and then "Manage Attachments". You need to make it a .ZIP file before you upload since the forums won't allow .bbcd files otherwise.

[blowncoupe]

OK I will give it a try

[jrmach]

On your file,you R/Click and pick send to compressed folder (that makes it a .zip)
In the posting area here,select "go advanced"
"manage attachments"
"browse"
select the compressed file and upload it.

[blowncoupe]

I hope this worked

[jrmach]

Well,here we go again....................Unfortunately it appears you have the latest update to V27.I only have the initial release on Demo.What that means is that anyone that doesn't have the latest update,can't open your file.And the only way to get the update is be on a maintenance($) plan.Hopefully someone can help.

[blowncoupe]

ok well thanks for your help

[jrmach]

This "Policy" BoB now has about one has to pay for updates is hurting users helping users on the forums.Since YOU just bought V27,you no doubt got the latest update.
I must Cautionanyone without the latest update to not try opening this file.It crashed really hard........I had to do a complete re-start of windows.Not no fault of OP's.
I never had that happen before,But now I am gun shy for sure.

Sorry BoB

[BurrMan]

Without looking at your file, my first suggestion is to look at your stock origin. Be sure it is moved to the bottom of the defined stock. Select the machine setup1 in the cam tree and note where the coord widget is.

[jrmach]

Since your new,I would recommend searching You Tube for video's
V25,26,&27 are in a lot of instances close to each other and are of value to learn from.
https://www.youtube.com/user/Depoalo...view=0&sort=dd

[BurrMan]

Previewing the file shows the stock origin kindof out and away from the defined stock, so be sure it is at the bottom level of stock...

The other thing noted from the preview is the stock is bound tightly to the part... A lot of the toolpath wont machine where there is no stock... Be sure there is stock for the tool to remove....

[BurrMan]

Here's a quick example with your surface where I added 1" of stock to both the x and y bounds.. This allowed a z level rough to go all over the place, as well as all the way down..

(I cant open your cam tree either, as I am on the original build, so just view this file to get the jist )

[jrmach]

https://www.youtube.com/watch?v=FadPCNItIk4#t=28

This should help along with what Burr was explaining

[RAF.]

One thing that I find kind of strange is how were you able to gen a tool path without any stock?. My download of your file doesn't show any stock or blanked stock. My program always has me run stock wizard before allowing me to continue on.

[blowncoupe]

yes I did go to the stock wizard first .I did leave the stock close though .I will try to run it with more x and y stock thanks for all
the help you guys

[mmoe]

One thing that I find kind of strange is how were you able to gen a tool path without any stock?. My download of your file doesn't show any stock or blanked stock. My program always has me run stock wizard before allowing me to continue on.

This is a known bug in V27. I spent a bit of time with their tech on this as I found my stock disappearing and it's pretty easy to work around. They should have it fixed sometime soon. If you open a file in V27 without already having another file open, the stock will often be missing. If you first open with a blank file (like the standard Bobcad1 file that is always there on startup), and keep the blank file there while you open the file you want to work on, the stock will show. My guess is that you happened to open it directly and there wasn't another file open already. Try it with Bobcad1 already there, then open the file and see if the stock appears (without closing Bobcad1).

[mmoe]

Back to the original question, most of the suggestions you've been given about stock and origin are spot on, but there is also one other thing to take into consideration when generating toolpaths. I don't necessarily agree that the machine setup origin needs to be within the stock bounds, but I do think it should be a location that makes some sense and was given some degree of thought. It should relate to the machine setup in a way such as a point that you can zero to on a vice, or the top of the stock, or something else that can be zero'd to on the machine and set up as the machine coordinates on your CNC. Since I can't view your original file outside of the part geometry (which I can merge into my older V27), I can't really say you did or didn't locate the origin in a logical place. My personal preference has become to zero my tool to the top of stock, so I typically place my origin at the highest Z value in the lower left X,Y corner. Others do it differently, but it shouldn't affect how Bobcad calculates the toolpath beyond how it generates code relative to that origin. Random origins won't work well in practice since you have to zero your machine to match, and it's hard to match random.

Also, there are settings that affect how the tool is positioned in relation to the surfaces you are cutting. For example, if you set the toolpath to "Bottom of Part" in the "Options" tab of the standard Planar toolpath setup, the tool will continue past the edges of the part (which it's using by default) and bring the tool all the way down until the widest part of the ballend touches the bottom edge of the part. If you change to a straight endmill, you'll find the toolpath does not go as far down with the same settings, but that's because it only has to go as far down as the part is deep, where a .5" ballend mill has to go an extra .25" to actually cut the full part. Sometimes it requires different options set to get similar results. If you're in Equidistant Offset, you may have to use the "Bottom of Job" setting to get the tool all the way down to the lowest edge of the area you want to machine. I just depends a bit on the toolpath strategy and the tool you are using. In the "Pro" toolpaths, there are generally more controls, but they also then require a little more experience to get them all working together right.

Wish I could be of more specific help, but it really is a challenge when I'm behind on the updates. I'll probably have to break down and buy a support package in January. It would be nice if we could somehow save backwards compatible files, but with the way the CAM systems work, that would be pretty difficult for Bobcad to ever achieve. The best we can do for now when the file is newer than the version some of us have here, is merge the geometry of the file, but that doesn't bring in the CAM at all.

[The Engine Guy]

If you have only very recently purchased V27 then unless things have changed dramatically you should have 45 days of free support from purchase/activation date, if you haven`t purchased a support package may I suggest you make the most of what free support time you may still have.

The support people are very good, they will "walk" you through stuff that is causing you issues, it`s usually a setting/strategy that you have/haven`t selected correctly, other than that as jrmach has suggested go watch the videos

Regards
Rob
:rainfro: :rainfro: :rainfro: