|
|
Post by joeblow on Aug 21, 2018 7:26:31 GMT -5
Not really sure about cnc etiquette here, but I'm hoping some of you with more experience than I (which is everybody  ) would be willing to take a look at my updated file for my 2nd attempt at the frame I botched up last week. Round 2 will be ready to mill in the next few days.
Here are some changes I made since my first attempt:
* cleaned up the corners for the 2 rail sweep * offset the inner and outer profile vectors by 0.05 for the final cutout as the first time around left skin on that would have been hard to sand out while retaining the final profile * originally I wanted the flowers to be 3d but didn't have that figured out last time so went with an engraving toolpath instead. This time around I have watched more training videos over and over and have attempted to create the flowers 3d * text is cleaned up but not sure if I should have used a quick engrave toolpath vs a vcarve/engrave toolpath * verified a hundred times that 0.3" is not 0.3mm 
File is too large to attach so I placed it in Google docs....
I promise that I won't hold anybody liable if it still doesn't come out the way I would like to see.
|
|
grg
Junior Member
Posts: 140
|
Post by grg on Aug 21, 2018 12:36:36 GMT -5
is that an Aspire file? Can't open it in V-Carve so it must be.
|
|
Deleted
Deleted Member
Posts: 0
|
Post by Deleted on Aug 22, 2018 8:29:39 GMT -5
If your tool path order is your planned cut order I would cut the inside before the outside. Also, when all is said an done you might be disappointed in how the text comes out, I would change to a 60 degree V-bit so it shows up better. I would add leads and ramps to the outlines. I would increase the text cut to 50-80 IPM and the finish to 70-100 IPM. For the roughing step, I'd increase the step over to 30-50%. You could cut your machining time dramatically if you used a square end mill to do the finish flat spots and the ball mill for just the detailed areas. For the outlines, I would also double the width of the cut for an inch or so. Since you're going down 1.7 inches you'll have a tough time evacuating chips if you don't make a larger channel than the bit itself. I would also add a last pass of 0.01-0.02 for the outlines.
|
|
|
|
Post by joeblow on Aug 22, 2018 19:20:22 GMT -5
Hi GRG. Yes it is an Aspire file. Thank you anyways for being willing to take a look.
Hi Fean. I appreciate you looking at this and responding. I mostly understood your advice. I will need to investigate how to separate the finish flats and the finish details for use with different mills. Makes perfect sense to do it that way just don't know how yet. First time around I did have problems evacuating chips for the outline cuts just didn't know how to deal with it besides chasing the cut with a shop vac. I will definitely add a relief channel this time.
|
|
|
|
Post by joeblow on Aug 23, 2018 5:43:58 GMT -5
Regarding the relief channel for the profile cutouts......not being able to see a way to offset the cut twice the diameter of the bit to a depth of 1” within the profile toolpath, my strategy will be to create an offset vector by .5” from the originals and then run a pocketing toolpath to a depth of 1”. At that point I should be able to run the original profile cutouts I set up with good chip evacuation. Regarding the “last pass”....really like that function and look forward to employing that in the future. I can definitely see how advantageous that will be but don't have a mill long enough in my inventory Still working on separating flats from details.. |
|
grg
Junior Member
Posts: 140
|
Post by grg on Aug 23, 2018 7:52:53 GMT -5
Sounds like something similar I had to do when milling this 2" thick maple. I drew a pocket out from the outside perimeter that was 3/4" wide for a 1/2" end mill (the end mill I had with the longest flute length on it). Worked fine for extracting chips.  |
|
Deleted
Deleted Member
Posts: 0
|
Post by Deleted on Aug 23, 2018 10:54:15 GMT -5
Regarding the relief channel for the profile cutouts......not being able to see a way to offset the cut twice the diameter of the bit to a depth of 1” within the profile toolpath, my strategy will be to create an offset vector by .5” from the originals and then run a pocketing toolpath to a depth of 1”. At that point I should be able to run the original profile cutouts I set up with good chip evacuation. Regarding the “last pass”....really like that function and look forward to employing that in the future. I can definitely see how advantageous that will be but don't have a mill long enough in my inventory Still working on separating flats from details.. Since your stock is 1.7" I'd go at least 1.25" and more likely 1.5" for the extra channel for the outlines. If you can cut 1.7" deep because you have that much stick out, then your bit will do a finish pass regardless of the DOC of the bit because it will still only cut the tool specified pass depth when doing the finish cut. In your outlines, you're doing conventional cuts but I would switch them to climb. Additionally, you can let the tool pick where it puts tabs but I never do, manually placing them means you can control where they go, thus make clean up afterward much easier. In your case, you can put them on flat areas instead of curves. I avoid right in corners but near one is okay, and prefer curve outside apex as opposed to inside apex. To clean the inside area you can have the tool generate an outline of the 3D model (modeling tab) and other features and do an offset from them, slightly more than the radius of your ball end finish end mill, and then use a pocket path with a square end mill. |
|
|
|
Post by joeblow on Sept 6, 2018 14:51:25 GMT -5
A shout out to Fean..Thank you for your suggestions and posts. Most helpful and appreciated. I employed all your advice except for the part about clearing out the flat areas separately from the 3d areas. i thought it be best to practice that one on a little less walnut |
|
) would be willing to take a look at my updated file for my 2nd attempt at the frame I botched up last week. Round 2 will be ready to mill in the next few days.
