contour problem

[shimmwagen]

i have a 7" long x .750 deep slot with a 1.06 rad at the bottom that im trying to mill with a .750 ball end mill. i think i drew the slot fine but now can't seem to get the toolpath sorted out...any suggestions??

thanks

using version 9...

[txcncman]

Can't open your file. Were you using a surfacing tool path? What were the results? Upload some screen shots.

[shimmwagen]

On the way home for the day. Was using contour tool path. I'll try to post file tomorrow.

[txcncman]

I think you will find it will work if you create a surface with the 1.06 radius and use a surfacing tool path.

[shimmwagen]

alrighty...i attempted the surfacing. Never done this with gibbs so hope i got this right. ill attach file again. if anyone wants to take a look and give their opinion that would be great.

[double a-ron]

Hi, I dont have Solid Surfacer and I think it's so funny when people who bought it use it to do things that can be done much quicker with simple "z machining" or in this case "x machining". A little known fact is that Gibbs will allow you to do simple surfacing without spending another 5 grand. It's called Z machining. Basicly you draw your conture, then tell it how far in z to machine it, as well as the depth per pass. In this case insted of machining in xy and steping down in z, I am machining in yz and stepping in x.

Here is how I did this:

1) Your model was upside down so I selected a face on the bottom side, right clicked on it, scrolled down to and clicked on "align face to cs". This fliped the part over and aligned it with the xy plane.

2) I went to the View menu and clicked "shrink wrap". This shrunk the stock to the model. Not really nessasary but, I like my stock that way and it's a cool trick.

3) I created a new CS by opening the cs list and selecting "new CS"

4) I opened the cs pallet and selected "yz plane"

5) Now I'm ready to get the profile of the slot, so I moused up to the top area where you can do things like turn on edge selection and face selection. I then turned on the "profiler".

6) I then selected the profile of the slot, right clicked on it and selected "extract profile". This turned the profile into geometry.

7) Then I deleted the unnessasary geometry, leaving just an open conture of the slot.

8) Next I created the conture prossess. The entry and exit fields will function normally, I prefer to rapid to .05 before the face of material but, you can put whatever you please. Feel free to review and play with the values I entered to see how they affect the toolpath.

The biggest thing to look for is in the "wall control dialog" located underneath the exit clearance plane. Notice how I tricked it into thinking I wanted a tapered wall? I did this so that I could take advantage of it's "back and forth" feature instead of having it do a pass then retract, rapid to the start of the conture and start again. To do this I simply left the all the taper and fillet control fields 0.

ENJOY!!!!!!!!!!!!!!!!!!!!!!!!!!

[double a-ron]

Here is another way...also done with no solid surfacer. This one is simpler but, the finish is not as nice. Review the file, if you have any questions please ask.

[shimmwagen]

im working with gibbs v9. any way you can save this so i can open it...

[double a-ron]

Here you go, by the way, copy is the second way I did it.

[shimmwagen]

thanks double a-ron. the way you did the part worked but i was having difficulty extending the toolpath past the part. i'll look at your file again when i have some extra time and play with it a bit more. i did end up using the surfacing option and ended up with a useable toolpath. some of the z retracts i dont quite understand, as in why they do what they do. i do have the manuals but cant seem to find much info that will help me, probably not looking in the right place.
thanks for the help and direction to all

ive attached my surfacing model, any feedback would be appreciated...

[txcncman]

Increase stock size to allow tool path beyond actual part size. Don't know why Gibbs does it that way, but it does.