Hello

I am in need of a vismill expert. I have had visual mill for a few years but have only used it for little pieces of code for small surfaces on some of my 2.5D parts. It has worked well for this over the years. I only use it a few times a year so I usually forget everything between jobs

I am tryinig to help out a friend and make some parts on my machine in my spare time and I am just having a hell of a time getting a "nice" somewhat efficient tool path.

I sent my file to mecsoft and the tech there masaged it and sent it back. I am running it now, but the roughing pass is barely adequate andthe re roughing pass cuts a lot of air. There is still stock at the bottom of the part which is not cut off.

The first coars parallel finishing pass dosent cut much of anything nor does the fine parallel finishing pass.

I have created tool path from meshcam and cut3d as well and while they are not perfect, I am much happier with the results.

You can see the meshcam cut part at: http://tinyurl.com/5cncmn

I will take a picture of the cut3d and the visual mill part once its finished cutting and post it here.

Is there an "expert experienced" visual mill user in the house that is willing to contract program this part for me so I can see what is possible with enough experience and knowledge of the software? If so please contact me at 562-477-2054 or email at grifftek @ grifftek dot com

You can see the files I have at www.grifftek.com/visualmill6

Thanks

Bill Griffin

You can see images of the part im trying to machine at:

http://tinyurl.com/687p5u

Thanks for looking

Bill

Bill-

That's an interesting comparison- I've never seen anyone post anything like that using a material that really shows the surfaces differences.

You may find that using the waterline finish option in MeshCAM will provide less scalloping in the vertical areas - at the potential expense of longer machining times. Just be sure to use the latest betas from the new section of the website since it gives more control over what areas are machined by waterline and parallel finishing.

-Robert

I think I see the problem: the part is vibrating because its fixtured on top of a keyboard :D

I think Rob has the right idea. A model with surfaces in various orientations like that requires different machining strategies to tackle different slopes. Parallel finishing passes are good for low (shallow slopes) and Z level waterline is good for steeper slopes and walls. How efficiently you can do this in VM, I don't know.

Another thing to consider is the accuracy of your machine. Older machines that can barely manage 200 or 300 ipm rapids tend to have significant servo lag. This has an almost 'backlash-like' effect when reversing directions on a slope, because one axis is a wee bit slower than the others, so this causes the tool to drag on opposite sides of the commanded position. This exaggerates the scallop effect above what the program actually should produce.

The workaround for this might be single direction machining when using a parallel finishing pass. I know, lots of rapids back to the one side, but you do what you gotta do.

Another thing to watch is the climb/conventional milling attitude of the tool. Conventional does not cut as clean as climb. If you are not actively thinking about what you are programming, it is entirely possible to be conventional milling on a sloped surface when it 'looks like climb' because the actual contact point on the ball mill may be on the wrong side of center. This all depends on which way you are stepping up or down the slope, relative to the tool travel and tool rotation.

Thanks for the responses. The machien I am running this part on is an Atrump B5AC with a Centroid M400 control with AC servos motors. Its 4 or 5 years old. I wont discount what you are saying about machine performance causing the surface issues.

I have the step over set for 0.020". I am trying to find a balance between time and surface smoothness. I can live with a textured surface more than I can live with an hours worth of time surfacing the part to get it smooth.

My problem with visual mill is I just dont have the experience needed to tackle a part like this. I keep banging away at it, but I am missing something. When I create a roughing pass, the tool cuts air all the way around the stock before it starts cutting the stock. I have tried all the various settings but I dont get what I want.I thik I have figured out that I need some sort of containment bounding region to force the tool to cut the stock but im not sure.

I need to try and keep the machining time down to about 25-30 min for the entire part.

Bill

You are right, Create the region and generate the toolpath inside it. You can select the two curves a circle or any rectangular shape as a region. This will help you. If u decrease the depth of cut and decrease the stepover i think the problem will be resolved.

i don't know why editing in the threads are not applicable????????


'decrease the stepover'

I am too busy to tweak your programming in VM.
I have programmed many parts with similar geometry configurations with very good toolpaths and part finish.

IMO - it is hardly fair to compare output of a program you are struggling to use with 1 that you are very familiar with.

On the other hand VM can be a bit trying at times. In my experience (when programming in 3+D) it is very important to ALWAYS use a tool containment region AND Z level upper and lower limits.
This WILL give you the cut areas required and DRASTICALLY reduce the computation time of the tool path.

It is important as well to import your part with fine faceting settings.
I always use "cut arc fitting" on parts like that as well. Been awhile for me but I believe you need VM Pro to do arc fitting in 3D finishing because I think it is done in the toolpath editor. (unless this has changed in V6 - I haven't done surfacing since I upgraded from V5).

Thanks for the response

I have not yet figured out how to create the regions, but I will figure it out when I get some more time on the program.

On the parts in the picture I am purpopsely leaving the finish rough or grainy like that to save on machine time as this is an acceptable finish for the part. I just spoke with my friend this morning after he seen all the pictures and he says its fine. The parts will be anodized and the look may be appealing to some and maybe not to others.

I have spent several more hours trying to figure out VM than I have meshcam or cut3d. I am new to all of these programs. It seems like you need to be a rocket scientist to figure out VM and a mere mortal can get decent output from meshcam and cut3d as they are very simplistic to use.

Does anybody have any programs they can email me that I can disect and see how you have programmed them?

You can email them to grifftek @ grifftek . com or put them somewhere I can dl them

Thanks
Bill

From the images, it appears that MeshCAM created the smoothest code? Is that what you see as well?

You can create the regions with the 'left side Menu', where you will find the tools like circle, rectangles, lines etc. Just keep ur model in top view and place the region (circle, curves, rectangles etc). then select the region and apply machining operation to that region.

Don't worry if the region is above the top of your model. It will automatically capture the projection under it and apply the machining operation.

Like Khalid says the Z height of the region is unimportant (this statement is NOT true if you are doing 4 or 5 axis work, but that is another story).
I am self taught on VM and the amount of CNC work we actually do here is often a couple of parts every few months (that is another story as well) point is my seat time and span between is WAY less than ideal causing me to have to relearn almost every time I open the software.
I am a blue collar tradesman and felt that I learned the software quickly and easily using the tutorials and making my own parts.

Just work left to right through the UI icons and you are done. Although VM6 has all the tabs to sequence through now, but it still works the same you just have to do left to right in 3 tabs instead.

I figured out how to use the super macro mode on the camera so there are a few more pictures of the parts as well as 2 more groups of photos of the part cut with a program generated in mastercam by my friend. The scallops will look like a feature on the part instead of a by product of a poor finish. The mastercam program runs 11 min with one finish pass and the cutter cuts very little air and there was only one un necessary retract between the final contour fininsh path which I could hand edit.

Now I need to teach myself how to duplicate his tool path in visualmill.

http://www.grifftek.com/grifftek/Machine_Work/machining_projects/AC_Tip/

Thanks

Bill

http://www.grifftek.com/grifftek/Machine_Work/machining_projects/AC_Tip/First_10_Parts/

Now I need to figure out how to make visual mill create the code that made this part....and make 160 more of them