Anyone have a simple method for indexing a piece so the contours on the back side can be cut? There are only two small raised edges to cut but I'm not convinced I can flip the block over and get Bobcad to hit the right spots. I've been doing it manually but thats not why I bought a cnc machine.
I would also like to know how to set up for finish cuts. I have been polishing the tool marks out by hand but these are very small parts and it would be simpler to just make a slow final finishing pass. I can't find much detail on finishing cuts in the manual and on the training dvd's. Oh yeah, I have V20.6 and Mach2mill. I am using the Fanuc6M post processor because the Mach2 post processor from the website absolutely will not work.
Finishing cuts are just like the other cuts without roughing turned on. Here is what I typically do....Raise the part by .003 in the cad Z. Do my initail cuts but add .006 to the tool diameter when posting. (this leaves .003 for all the surfaces) Lower the part in the cad by .003 and post a finish cut but only go .002-.003 stepover, all the tolerances as tight as it will allow and no faster feedrate than the machine can handle.
Doing it that way usually gives me a finish I can live with but on very tiny parts you may need to play with it a little more.
As far as flipping the part you will either need to get fixtured or buy a 4th axis.
Tjones method will work I use a little difference approach when I program tool path I will use the same tool and just change the value of the tool either in the profile or with the planner path with two different colors that way I know which path I want and in the attributes on the general page I will name it by the dia. I programmed so when I get to the cam side I can either call the path by color or layer as for flipping and hitting the mark thatís controlled by your cad skill and machining skill Bobcad will hit the mark if you tell it to
Thanks T and Mike, I follow you both most of the way but I have one question. How do you incorporate both files? Will the NC generate and stack two toolpaths/layers or do I merge them myself somehow? As for indexing, I was afraid you would say that! I guess I'll make mass quantities of chips until I get the cam side down. I appreciate your insight.
Anyhow programming and the use of them is really determined by the person who does it. There are 101 way to get there but I can tell you a couple I use. I also make my paths different colors but have lately not even saved the path on the cad side as it does me no good after it is generated and I can always make it again from the cam program.
BTW...my way of offsetting is because I may use a 3/4 ball to rough and a 3/8 to finish and so on or even a bull nose carbide insert mill for all. I post using the tool tip instead of the center due to the different tools and not confusing the guy setting up the machine.
So to answer the question about roughing and finishing.....I do it both ways. Why? Because on some of my jobs the program will run for around 20 hrs or more and we run it during the weekend or overnight. So a few good points and bad. First you can combine them by simply making the roughing cut and then, if needed, a tool change and then the finish cut. Bobcad does this easy.
Good ....can run unattended....bad...will need to sepperate for re-running finish cut if needed.
Sepperate programs are good for manual tool changing if you dont have a tool changer. Sepperate programs give you the chance of seeing what went wrong on a settup. Also hard to change just part of the program to say modify one section....I always place a marker line of text stating something like 'semicut start position'.
Combined program lets you simulate rough and finish cuts together. Lets you send once and run complete. Run overnight or weekends etc...
Anyhow programming and the use of them is really determined by the person who does it. There are 101 way to get there
That the key there, once you have your cad file and save it you can do your code to fit your needs. So when you run the cam side is where the cad file comes in. The machine you use today may not be the same you use next time example Matuura 1500 1994 machine can read a G12 or G13 same machine made a couple of year early can't read a G12 or G13 both machine can read a G2 or G3 that why Bobcad will run EIA stander format. You cad file is the one that has to be set up the way you need . So labeled layers and colors can be very helpful as long as you know what they are.
LOL, I appreciate the simplicity of your explanations. You two are well beyond my current abilities. I get a thrill when something goes right for me! I think I'll give the tool change method a try. If I use the same row of home code, will my tool return to the original starting point? I have also been reading that you can use "profile" from the NC menu to make a finish cut but your methods make more sense to me at this point, Here goes nothin', maybe less.
On most machine when the M-6 is called up the spindle will return to Z home, x and y will stay the same. Just keep play around with software and you'll be a pro in no time. You can send the code to the machine and just run the graphic function if your controller has it. If you have a code issue it will tell you also you can visit Bobcad Support site for some other post. On the cad side go to help there a direct link for you in the software. Best of luck and ask what ever you need to know there are a lot of us that will take the time to help you
The type of cut you use is determined by your job. 95% of my work is solids contouring(3D machining). The path for solids is done in the Solids menu of the CAD screen.
If you do pocketing or profiling(inside or outside) then you can use the profile from the NC window.
There is so many types of jobs and cutting that most people will never see them all. This is why it is hard to answer a post that might say...."I have a part to make can someone tell me how?" That post may never get a reply!
There are some videos available by Sorin (the one who does Bobcad training courses). Look in the post about tutorials and see if they are still on the free sight. They get removed after a while (free after all).
I guess I'll have to check those out. I have been at it most of the day and still have not gotten to the finishing cut. This is a 3d drawing but I'm about to the point of confusing myself. I am apparently not combining the tool paths and somehow overcompensating for my cutter and taking too much off. I working on my sixth variation of your suggestions right now. I thought I could follow directions. At leasy I changed the waterpump on my van while my machine was cutting.
Are you removing too much in Z? Or is the sides or both? When posting the path using the solids menu make sure you select the correct path representation ---tool tip or tool center(only ball tools here).
The cutter type musy me correct as well. Don't select a ball if you are using a bull nose.