[aaron p]

Hi All,
I spent 2 years learning CNC and programing at a small high precision (titanium/inconell) shop doing oilfield work. My old boss let me learn 3axis milling on EZ-Cam running Fanuc controlled VMCs. Ive since left the shop to move to a bigger company making much more money. Well anyway, I have a buddy thats willing to give me a Mori-Seiki MV-35 VMC. Its a little rough, but it all works and has the Fanuc controll im used to. My questions are, can I import .jpeg images to create tool paths to engrave logos and such? Is there a way I can use different fonts do engrave text on EZ-Cam? I havent bought the software yet or even gotten the mill yet, but just trying to get some ideas in my head. Also, is it possible to machine O/D threads on a round male part on the 3axis? Heres a picture of kinda what im talking about.
http://static.summitracing.com/globa...-mp-6266_w.jpg

IF not, how would that part be made on a 3 axis or would it have to be 5axis of some sort?

[nanopile]

Well, it wont look that good from a picture, you need the cad data.
You can propably import the picture to a cad program and then make some kind of heightmap and then use the cad data from it to generate G-code.

[idaho psycho]

bobart, which is a part of bobcad, has an import feature that does that,
many other programs do also. I don't know anything about ez cam, but maybe you could open your file with a program like bobart, and then save it as a cad file to work with in ez cam. a friend of mine imports the file to his cad program and then basically traces the pattern manually (in the cad program) with lines and arcs to come close, works good on simple stuff, but a pain in the butt for complex work

[harley4ever]

bobart=artCRAP

[idaho psycho]

bob cad has some aspects that are definetly cheesy, but for the price of it, it is hard to knock, I have done a lot of work with it over the years and it has paid for itself many times over. if you call them you can purchase it for much lower than the prices they advertise in the magazines. it doesn't compare to the expensive ones (other cad programs), but it is good for beginners that don't want a hack copy of a more exotic one.

[Paulo E.]

Aaron, look for a program that converts "RASTER TO VECTOR" that is the correct terminology. As someone pointed out bobcam I think may offer that feature, many others might do the same or better. I will attach a link that might help you. Some of this programs are free so dig in at your own pace. As for the threads, yes you can do them in a VMC as long as your cam software outputs the code or you can actually do it by had, there's nothing to it, really!!!

http://en.wikipedia.org/wiki/List_of...rsion_software

Hope this helps you and good luck with your new machine

[dradef]

Not sure if it is what you are looking for - I have used a very very basic software called "BMP 2 CNC" - it takes an image file (not just .bmp) and converts it to a "heightfield" using the grayscale of the image, then creates a toolpath directly in the software, no need to send to seperate CAM software.

For example, black can be set to the concave areas and white can be the high areas (or vice versa), then any shade of gray between black and white will be a height proportionally between the low and high based on how dark or light it is. For clarity, I will attach a picture I just took of my first example of a logo that was machined into a block of plastic using this software (posted to a haas machine, using a .0625" ball end mill, then sandblasted). I will also include a small example of the image file used to get these results.


As you can see in this example I set the dark as the "high" and light as the "low". The elliptical shape surrounding the text has a gradient from dark on the left to light on the right which is translated into a smooth ramp from the light to dark areas. The details are also picked up, like the little horizontal lines that run through the large text and also how the main text is slightly darker than the elliptical surrounding shape making the text appear to sit on top of it.

Keep in mind it is very basic software. It is also very cheap (I think $20-30 to purchase the full, unrestricted version) so not much is to be expected. Some images will have better results than others. Sharply defined edges are a big plus.

Hope this helps.

[bk1955]

I used EZcam for years to make clicker dies for various labels. I used a software called Image Invect. I don't even know if it is still around. You have to use something to scan the drawing and then use a software to convert it fom raster to vector. It was actually raster to dxf format. The thing is that most of those conversion programs work well with a skinny line, but not with bold or wide lines. I have done this lately once with another conversion program called Cutting Shop, but I didn't use it enough to get good at it. The bottom line is that you can't put something in and have it spit out what you need. You will have to edit it and it will take some time.

[jetpig1]

Well anyway, I have a buddy thats willing to give me a Mori-Seiki MV-35 VMC. Its a little rough, but it all works and has the Fanuc controll im used to.

Wow, now that's a REAL buddy !

My questions are, can I import .jpeg images to create tool paths to engrave logos and such?

No, you need some sort of CAM program to do this on a Fanuc.

Is there a way I can use different fonts do engrave text on EZ-Cam?

Not sure on Fanuc, FADALs have some, again a CAM software package with vector tool paths. Vectors are just a direction and a magnitude, meaning which way, and how fast. Engraving is very common and very simple on a multitude of CAM packages. Pictures can be imported, although in this case I don't think you need it, and a raster to vector routine would be used to get toolpaths. Most employ high/low geometry from light/dark areas of a bitmap.

I havent bought the software yet or even gotten the mill yet, but just trying to get some ideas in my head. Also, is it possible to machine O/D threads on a round male part on the 3axis?

Sure, a threadmill can do that operation, basically machines a helix around the material. Clearance could be an issue.

IF not, how would that part be made on a 3 axis or would it have to be 5axis of some sort?

3 axis would be enough, with some creative fixturing, perhaps a 3 or 4 stage setup could get ya there....Good luck, and thank yer buddy for the nice toy...

[email protected]

[VWSatOz]

to make threads on a VMC I have used the SPIRAL milling function of Fanuc on a OMA control. This required each thread whirl full circle to have its own line of program, ie a G02 or G03 plus the Zdepth increment =pitch of thread ( for a vertical down spiral )
I was in effect "tapping" into drilled holes in a very hard bronze type material using a single point fly cutter made from solid carbide, small enough in diameter for the tip not to hit the other side. I called it thread whirling. Tools are now available with full thread form of various pitches. These were internal threaded holes.
To mill three external studs as your picture shows you would need to hold the work upwards & mill around to create the male shape using mills & angled form cutters for the tube flares to seat onto. Then thread whirl around the outside male round to cut very accurate threads. (or use a die nut in a floating holder and the tapping cycle).
You would then have to index the part to the next leg of the Y and repeat all above.
The engraving can be done using EzCam & tablet but I have never been able to import data so it takes a lot of work. I made my own set of letter & number fonts and move & enlarge rotate to suit, very laborius! I have an old version of 2D EzCam on 8" floppies! runs on 1983 NEC HO3 PC that I still use and love it!

Of course a lathe would be much simpler! with index fixture on a face plate?

[kdhBOSS5VRAM]

Wow, I'm glad to hear someone still uses that old EZCam system. I wish I had one. That's what I learned on in the early 80's, in fact I still have the 8 inch floppies in my toolbox. As far as engraving, what I've used is Bobcad's BobArt because I can scan a logo and then use BobArt to make a geometry file. From there I import that into EZCam and make a path out of that from the geometry file. There are probably a lot easier methods, that BPM 2 CNC one looks interesting and I think I'll try that. I know EZCam has a program, I think called EZText that you can do all of it on but we don't have it, just a demo. With the newer versions of EZCam you can do simple text easily but can't alter the fonts, good for basic lettering but not much else. Beats trying to draw each letter out though.

Kevin

[aaron p]

Not sure if it is what you are looking for - I have used a very very basic software called "BMP 2 CNC" - it takes an image file (not just .bmp) and converts it to a "heightfield" using the grayscale of the image, then creates a toolpath directly in the software, no need to send to seperate CAM software.

For example, black can be set to the concave areas and white can be the high areas (or vice versa), then any shade of gray between black and white will be a height proportionally between the low and high based on how dark or light it is. For clarity, I will attach a picture I just took of my first example of a logo that was machined into a block of plastic using this software (posted to a haas machine, using a .0625" ball end mill, then sandblasted). I will also include a small example of the image file used to get these results.


As you can see in this example I set the dark as the "high" and light as the "low". The elliptical shape surrounding the text has a gradient from dark on the left to light on the right which is translated into a smooth ramp from the light to dark areas. The details are also picked up, like the little horizontal lines that run through the large text and also how the main text is slightly darker than the elliptical surrounding shape making the text appear to sit on top of it.

Keep in mind it is very basic software. It is also very cheap (I think $20-30 to purchase the full, unrestricted version) so not much is to be expected. Some images will have better results than others. Sharply defined edges are a big plus.

Hope this helps.

Thats exactly what im looking for. Where can I purchase that software? I like the Dark/Light setup. Makes it easy to see. If I can get it to a .dxf format, I can load it into ez-cam and write a tool path. Does this software have a post processor?

[aaron p]

Also, where can I get a die holder with a floating head for CAT 40? I think using a die on a threading cycle would be easiest as long as the machine could thread up to 1.062"-12TPI thread.

[dradef]

Thats exactly what im looking for. Where can I purchase that software? I like the Dark/Light setup. Makes it easy to see. If I can get it to a .dxf format, I can load it into ez-cam and write a tool path. Does this software have a post processor?

The software is from a company called MR-Soft and can be found at www.mr-soft.net

I think I counted 38 post processors in the most recent release. They are all included in the download so you don't have to search for the one you need to add on. I know they offer a functioning demo, but it will only output a maximum of 150 lines of code.

The BMP 2 CNC software can't save the resulting heightfield as a dxf. It is solely to turn picture files into g-code. So, if what you are saying is that you want to use your own CAM software to make the g-code program you might look into their other sotware called "R2V" (this is a raster to vector converter, like has been mentioned by others. i don't think this method gives 3d results though.) R2V specifically states that it can save as dxf.

I looked up the newest prices. They are both around $44.00

I don't think I paid that much about a year ago when I decided to get it. There might be cheaper alternatives.

[aaron p]

awsome. Thats exactly what im looking for. Ill pick it up and play around with it untill I get my mill setup and such.

[aaron p]

Just got the software and allready made a bunch of NC files. Now, how can I convert that .nc file to .txt or something that I can put on a floppy and send to the machine to read? Its a fanuc O-M control I believe.

[dradef]

Just got the software and allready made a bunch of NC files. Now, how can I convert that .nc file to .txt or something that I can put on a floppy and send to the machine to read? Its a fanuc O-M control I believe.

You can put the .nc files on a floppy. On our Haas machines you would just have to enter "yourfilename.NC" when loading the program.

If your control requires it to be a .txt file extention you can open the .nc file in notepad, then select "save as", then next to 'save as type' select "all files" then in the 'file name' box add ".txt" to the end of the file name.

Also, these types of contouring programs tend to get larger than a single floppy can hold. If your control has enough memory to hold the entire program then there are some very easy tricks to work around loading chunks of the program from multiple disks and still running seamlessly (even if the control can't hold the whole program it can be done, just not quite as easily).

Let us know.

[VWSatOz]

The EzCamII on old NEC APC pcs are a monster, so heavy can barely lift w/out the back popping! Have 1 at work & spare at home, but home1 has blown the high tension transformer on the VDU board and having lots of trouble getting mates to try & fix it or hooking up to different screen altogether, have been given an NEC multisync to try this way later if I'm game. Used to be able to program at home late at night & take 8" floppy to work and mill away! & need the 2 antiques as backup as wont run on anything else.

[aaron p]

You can put the .nc files on a floppy. On our Haas machines you would just have to enter "yourfilename.NC" when loading the program.

If your control requires it to be a .txt file extention you can open the .nc file in notepad, then select "save as", then next to 'save as type' select "all files" then in the 'file name' box add ".txt" to the end of the file name.

Also, these types of contouring programs tend to get larger than a single floppy can hold. If your control has enough memory to hold the entire program then there are some very easy tricks to work around loading chunks of the program from multiple disks and still running seamlessly (even if the control can't hold the whole program it can be done, just not quite as easily).

Let us know.

Worked like a charm. And you aint kiddin about programs getting long. I was playing around with a detailed logo and it was around 28,000 G-code lines. A 2,300 line program is only a 120KB file in note pad. Not a problem for the controll. thanks a ton guys!

[kdhBOSS5VRAM]

We used that old EZcamII V2.4 system for a lot of years, even back then we had a spare terminal I had to scavenge parts from. I really liked using it and I remember it was a big step to go to a PC with Version 6. We currently use Version 14.5. Are you able to even still get them 8 inch floppies and have you tried the newer versions of EZCam?

Kevin