Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: Overloaded on March 24, 2013, 04:08:15 PM
-
Hi folks,
I have a block that I wish to machine a "tapered to straight" radiussed groove into with a .050" ball endmill.
Attached is a basic 2 view dwg of one similar.
How do I go about creating a toolpath for Mach and my mill ?
I might figure it out with MeshCam, but first need a "model, 3D drawing" or something ?
3D is a new one for me, any help welcomed.
Thanks,
Russ
-
Well I can suggest a 2 1/2d approach but I am not a very active user of 3d solid modelling and 3d CAM (real old school).
(;-) TP
-
???
-
???
-
Hi, Russ
Well, when it comes to 3-d I am a 1-DUH guy!
Guess my approach to this would be too simple and probably wrong, but looks like it would produce a tapered line starting at y0 z-.05, moving to y.75 with z moving up to -.0285 as it traverses (should give you a taper and the radius you want) then cutting the last .25 inches at -.0285.
I am assuming as you stated that you have the cube. If not, then I am completely wrong (not unusual).
Bob@BobsShop
-
Yous Guys are 2 fancy for me(;-) I did do a sample of 2.5d workl to show its use. I did it in MAch3 conversational(;-) Of course it needs to be adjusted for use.
Being all the angle changes are linear it would be a piece of cake for a Parametric SUB
(;-) TP
-
this might work for ya
-
Wow ... Thanks for the attention guys !
Hi Bob, you can more clearly see what I am wanting from the other replies, thanks for your input though as that is similar to what I thought at first. :)
TP, I may have several of these to do. I might hit you up for a Wizard for this parametric thingy, and/or a good tutorial, thanks !
YNN, Perfect ! Until I get the .05 cutter from Bits&Bits, I will run your file scaled up and use a .125 cutter that I have.
Rhino ... happy with it ? Is it CAD and CAM ?
Thanks again so much men,
Russ :)
-
BTW, the material is A2 or 0-1 tool steel.
? Is it possible to do all of the cutting in the longitudinal direction ?
roughing it down, then shallow stepovers for the finish passes ?
Thanks guys,
Russ
-
Rhino and MadCam
took less than 30 minutes including drawing the 3d surface layer to drive the cutter path.
imported the dxf for the line endpoints.
I set the step over at .010" per pass.
Used a function button named, drive cutter path between two lines.
picked the two angled lines that were previously joined to the two straight lines.
then picked the two radius lines from the angled section
then the two radius lines on the straight section.
then arranged the layers in the way I wanted it to cut.
layer order is the sequence of operation.
move the order, change the cutting path sequence.
Fun programs to learn and very powerful. 8)
while I was composing this, you posted:
this is "post processed" as stated above in both directions as you want.
I assumed it was for tool steel.
-
Thanks a bunch Craig ... much appreciated !
I'm anxious to scale it up and try it later today.
I was asking if it would be feasible to do ALL of the cutting in the SAME direction ... longitudinally.
Maybe not recommended ? for some reason ?
It will be polished 9 .001-.002")after machining.
Cheers,
Russ
-
EDIT ........
It will be polished (.001-.002")after machining.
Cheers,
Russ
-
I used cut in both directions to minimizes the step over ridges that are created. But I might run a single roughing pass thru the center line to clean out the mass leaving ~.010"-.015". Easier on the small cutter flutes. Looks like a sprue. Have fun polishing.
-
Yeah, I see the fun coming up.
I got the Rhino5 user guide and am looking through it.
Great explanations in the begininning, thanks again Craig,
Russ
-
While waiting for the .050" carbide ball endmill to arrive, I used a HSS .125" one to run a simulation/model in aluminum.
I scaled the file up 2.5
Came out quite well. Little effort polishing, but realize that will be different with the steel.
All in all, I am pleased. :)
Thanks guys, will be back to learn more later ....
Thanks again,
Russ
:)
-
Good Job Guys, (;-) TP
-
Well ain't that purrrrdy!!!
good job Russ
-
Little effort polishing, but realize that will be different with the steel.
I would reckon that your polishing woes are largely due to the fact that you cut a scaled up version, hence a larger step-over.
Rhino is really a superb program. Great price for it too, or it at least it used to be when I was looking into it. It is a very advanced program though, so the learning curve is quiet huge, as is the rewards once you get a firm grip on things. There are quiet a few CAM programs for it, so no lack of choices in that area. Chris Botha uses Rhino with DeskProto I believe. We all know the wizardry and magnificent jobs he accomplishes (i think he sold his soul for those skills), but he's not exactly a weekend warrior, either.
http://www.machsupport.com/forum/index.php/topic,11446.0.html
http://www.deskproto.com/
Side story:
I know that book all to well in the background.
Dad:I've been reading these westerns for quiet a while.
Me: Really? That sounds nice.
Dad: Oh it is! Let me tell ya, they really get interesting at times! Six shooters! Trains! Indians! Gold!
Me: : ::) ::)
Dad: You probably wouldn't know a good book if you picked one up. I bet you haven't even opened one up since you were in school.
Me: I read. I read allot, actually. Just yesterday I read a few pages of a real good book.
Dad: I bet. What was the name of it? Penthouse?
Me: ;D No. Penthouse is a magazine. Ain't no words in a Penthouse anyhow. Just pictures far as I can tell. It was called McMaster Carr.
Dad: McMaster Carr? The name certainly sounds interesting. Kinda got a western ring to it. Any guns or train robberies?
Me: No. Maybe a strongbox or a knife or two, though.
Dad: ::) ::)
-
:D ;D
Thanks Sam.
I'm anxious to try it with the steel and proper cutters.
I'll post the finished part if it works out right.
See Ya,
Russ
:)
-
Hi folks,
I have another request.
I am trying out a demo of MeshCam.
It can open an STL file but I have no way (afaiko) to produce one.
I modified the earlier project a bit and wonder if someone here would mind to take the attached DXF and convert it to STL for me.
Everything is drawn to scale so all of the pertinent info should be there.
After MESHCAM, if I can get it to work for me, I will need to figure out what I need to do the dwgs.
Thanks,
Russ
-
STL's are 3d. DXF's are 2d. No worries, simple enough to draw out.
There are many options for exporting to STL. There are also many options for importing. Half the battle is finding out what export and import settings "jive" together. Sometimes it's good right off the bat, sometimes it can be a pain. Anyhow.... see if this is what you need.
-
Also, you might wanna give Autodesk 123D a try. I tried it quiet some time ago, and it seemed to be VERY capable. It did not do something that was a necessity for me at the time, but I can't even remember what it was. Probably sorted by now.
Taken from the website
What's new in this version: export STL, inserting models to an existing model, sketching enhancements, dimension tool, send to CNC utility, other minor enhancements, bug fixes.
http://www.123dapp.com/
http://www.123dapp.com/design
-
Hey Sam, THANKS ! :)
What prgm did you use for the conversion ? (if you don't mind sayin')
I'm anxious to run this if MeshCam would hurry up a bit and send my registration code. Been 4 hrs.
Oh, thanks too for the links.
Looks like my hdwre isn't capable though.
I'll keep ya posted of my progress.
Thanks again,
Russ
-
Software is solidworks. What a bummer about the cpu requirement! I wouldn't have thunk it needed those specs. Where ya falling short? Win7? I wouldn't think you would need an internet connection just to use the software.
-
Hey Russ,
Attached is quicky how to on using ACAD and Meshcam.
RICH
-
That's EXCELLENT Rich ... THANKS !
I might try to get my boss to buy AC for me, that would be great.
I did get the MeshCam registered, went through the tuts. and HELP files.
It's pretty basic, easy to understand and work with.
The first sample I did was in alu using the Parallel in X approach, just like you illustrated. .0015 stepover.
Did a great job but leaves the very small scallops on each side of the profile ... just as you see them in your MeshCam post-machined model.
Then I did one utilizing the Waterline method and it came out much better in that there is only half of the polishing necessary due to the scallops, or steps, only being in the bottom of the trough, none on either side.
Here is a sample I just cut, actual size with a .050" ball endmill in 0-1 tool steel.
.0015 stepover, about 4 ipm, 20,000 rpm.
Very little to polish, 5-10 minutes using a stick with lapping compound.
My machine has about .0006-8" backlash or the results would probably be a bit better.
ALA in all .... I think it will work.
Thanks for all of the help ... all of ya.
Russ :)
-
Looks good Russ,
Have a look at the attached about stepover values.
Note that most of the info came from a posting on the Mescham site by Robert.
RICH
-
That is a SUPER read Rich, thanks !
Especially interesting is the Surface Angle Limits feature. That's one item I was wondering about but had not seen a concise description of.
I checked to find that I'm actually stepping over .002" .
I started to go with .001" but felt that the cutter would hold up better taking a bit of a bite rather then rubbing off the lesser amount.
Anyway, Here is a pic of a pair fresh off of the mill, as milled and untouched.
There is also the alu sample run and the 0-1 sample that has been polished and heat treated.
You can (I hope) clearly see the small scallops, only in the very bottom. 10 minutes each and they are polished up slick as a whistle.
Dang, that .050" ball endmill looked sooooooo small ....... till I took out the .025's. Jeeeeesh, maybe I should just sell them cheap before I bust em' up. ::)
Thanks again Rich,
See Ya
:)
-
.... ooops, the treated one is not in that pic.
Russ