cnc and Bobcad

M

mcconecue

Registered
I have finished building my cnc machine, and going thru the learning process. I have Bobcad v21 and Mach3. The problem I'm having is getting inlays to fit my pockets correctly.

Since this is V.21 I am having what seems to be a hard time finding a good post processor. I also may have something set wrong in Bobcad.

Cnc is all new to me but I know I will figure it all out. I know my problem has to do with tool comp. or offset but cant seem to find the answer to pocket fit.

I am looking for any info on posting and assistance in using Bobcad V21. I feel I will upgrade V23 at later date, But really want to learn and test this machine before the cost to upgrade.

Any assistance will be greatly appreciated.

Thanks
MCC
 
mcconecue said:
I have finished building my cnc machine, and going thru the learning process. I have Bobcad v21 and Mach3. The problem I'm having is getting inlays to fit my pockets correctly.

Since this is V.21 I am having what seems to be a hard time finding a good post processor. I also may have something set wrong in Bobcad.

Cnc is all new to me but I know I will figure it all out. I know my problem has to do with tool comp. or offset but cant seem to find the answer to pocket fit.

I am looking for any info on posting and assistance in using Bobcad V21. I feel I will upgrade V23 at later date, But really want to learn and test this machine before the cost to upgrade.

Any assistance will be greatly appreciated.

Thanks
MCC
Click to expand...

Do some test pieces and sometimes you have to lie to the program about the size of the cutter to get the proper fit. Keep experimenting with telling the program slightly smaller or larger cutter sizes until you find what gives you the best fit. I have had to re-cam all my programs several times when changing from one spindle to another because the more precise your spindle, the closer to actual cutter size you can tell your cnc program. Often I have found it where I've told it I used different sizes for the part & the pocket. For example when using a .0312 cutter I might give the program .0290 for the pocket and .0310 for the part. Once you get the right combination, it should stay constant until you burn up a spindle or laminate trimmer and have to go through the whole process again with the replacement until you get the proper fit.
 
Just a few thoughts.

mcconecue said:
I have finished building my cnc machine, and going thru the learning process. I have Bobcad v21 and Mach3. The problem I'm having is getting inlays to fit my pockets correctly.

Since this is V.21 I am having what seems to be a hard time finding a good post processor. I also may have something set wrong in Bobcad.

Cnc is all new to me but I know I will figure it all out. I know my problem has to do with tool comp. or offset but cant seem to find the answer to pocket fit.

I am looking for any info on posting and assistance in using Bobcad V21. I feel I will upgrade V23 at later date, But really want to learn and test this machine before the cost to upgrade.

Any assistance will be greatly appreciated.

Thanks
MCC
Click to expand...

Your post is a little too vague to know how to answer, but I'll offer one suggestion off the top of my head.

One thing that can drive you crazy when you're trying to get inlays to fit correctly is backlash. Have you checked the backlash on your machine? Are you using MACH's backlash compensation?

Outside of that, I have more questions than answers.

I don't understand what you mean by not being able to find a "good" postprocessor. What is your postprocessor doing (or not doing) that is causing a problem?

You also state that you may have something set wrong in BOBCAD. It's possible, but I have no idea what you're refering to with this statement.

If you could be more specific, I'll try to help if I can.
 
cnc

Yes my question was pretty open and vague. I did not want to write a book here on the forum on every thing I have done to this date.

Yes back lash has been tested and is almost dead on. Spindle run out is is not a problem. I'm using an Nsk at 30,000 rpm.

Now the copy of Bobcad I have came with an older cnc I purchased. there are 5-6 post in the system . The ones I tried have some issues in posting, Some do strange things like always inputing G41 and G40 even when tool comp is off. Then if i try to program in an offset it throws the part size way oversize.

So I know its just my lack of knowledge in the software .

I also was hoping somebody can suggest what post processor to use .

Also looking for correct way to cut pocket and parts for best fit.(IE) what size finishing pass to make ETC as this is all new to me and just learning. So anything on correct procedures for pocketing will greatly be appreciated.

Thanks Sherm, I will do some testing on changing the tool sizes and see if I can find the right fit.

Thanks
MCC
 
mcconecue said:
Yes my question was pretty open and vague. I did not want to write a book here on the forum on every thing I have done to this date.

Yes back lash has been tested and is almost dead on. Spindle run out is is not a problem. I'm using an Nsk at 30,000 rpm.

Now the copy of Bobcad I have came with an older cnc I purchased. there are 5-6 post in the system . The ones I tried have some issues in posting, Some do strange things like always inputing G41 and G40 even when tool comp is off. Then if i try to program in an offset it throws the part size way oversize.

So I know its just my lack of knowledge in the software .

I also was hoping somebody can suggest what post processor to use .

Also looking for correct way to cut pocket and parts for best fit.(IE) what size finishing pass to make ETC as this is all new to me and just learning. So anything on correct procedures for pocketing will greatly be appreciated.

Thanks Sherm, I will do some testing on changing the tool sizes and see if I can find the right fit.

Thanks
MCC
Click to expand...



What you need is a post processor for mach3
http://www.machsupport.com/posts.php
click on the POST beside bobcad-cam to down load post
if this dont work give me a call and I can get you the post that you need
 
cnc

Thank you all for your response. Thank you also Joe for you offer . I will give you a call, Thanks to all the PM's. I'm sure with the help that has been offered I will be able to work thru this.
 
Would think the people at Mach3 could help you with a post processor.
Call Jim at Unque Products ... he can fix you up with a post processor for BobCad and Mach3.

I dont use tool offests ... I keep it as simple as possable.

Here is how I do my inlays with BobCad 20.

Lets use a simple oval as an example.

I draw the contour line in black.
I then use the Other - Pocket - Spiral program to draw the tool path lines inside the oval in blue.
I number this and add the leter A -- 015A -- the A signifies it is a pocket.
NC is used to generate the G-code.

For the inlay piece I delete the blue lines then rename the drawing to 015B - the B signifies it is an inlay piece.

I choose Other - Offset - and draw a line around the inside of the oval .003" smaller and make this line black.
I then delete the outer black line.
Now the inlay piece is .003" smaller than the pocket.

Next I do Other - Offset and draw a line around the black oval, offset by the radius (not the diameter) of the tool I plan on using.
I repete the offset on the line I just made and make those two outer lines blue.
They are the tool path lines.
I break and connect the two blue lines so they become a tool path around the outside of the oval inlay piece.
Next the piece is copied and pasted to make a drawing with many of them nested and then connect them with dotted red lines to make one continuous tool path.
Again NC is used to make the G-Code.

This is what works for me.
 
Last edited:
your help appreciated

Thank you Willee.
Your procedure worked great.

With all the help here and in Pm's and a great processor sent by Lee, the pockets and parts are right were they need to be.

Again thanks to AZB forums and the great people and the knowledge they share here, my struggle of weeks on end fighting this problem , was solved in one day in the shop armed with the info given.

Again thanks to ALL who responded. :D
 
glad things worked out for you some may disagree but 21.5 works great even though i have 23 i haavent really used it jim(mc2) likes 23 and is very good with it my fortee is 21.5 i just wish i had the time to use it hopfully this winter i will good luck and please post some pictures of your inlays
 
Another thing to keep in mind, is that your cut direction, and how much material you are taking off will also affect the sizes of your parts and pockets.
I tend get the best results with a 3 to 5 thousandths finish cut, ccw for parts and cw for pockets.
 
You must log in or register to reply here.
Back
Top