Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.
I did try that one but it has trouble with arc moves. And I can't get it to work proper after editing. The AGE 3 control I am deaing with is very basic. It uses an "R" code instead of I,J,K. I am assuming this means it does not use circular interpolation. ProE tech support told me to start with a Fanuc 1 post file and edit it. I have no idea where to even find a Fanuc 1 post. My ProtoTRAKmanual is telling me the control is similiar to a Fanuc 6 post.
Does anyone have any idea of what machines use a Fanuc 1 or Funuc 6 on our list of posts from our ProE post library?
Hi Tesla,
The "R" means it is replacing the I,J value in the X,Y plane. It probably does perform circular interpolation, hence the "R".
I would try the FANUC 6 post and where you're outputting I,J you want an R. Fanuc posts are probably the most common. Find any machine with a Fanuc control and it will still probably output for a 6 series. There may be some newer G codes for Rigid tap that the 6's did not have, but the basicG code set is still the same.
Send me some output from the posts you're using, maybe I can help.
G-code output - Current and what you NEED. We can work on the wants later.
CL data, NCL data, and a pdf manual, if available.
As Jcrook Says it doesn't use IJK output but that's an easy change in the post. If you open the post with the option file generator.look at the left side for motion and click it to expand it. In the pull down list you will see circular. Click circular thenyou will see in the top middle of the page crcle center output with a pull down list.that isset to output IJK now if you pull down the list select output radius then save your changes. That will switch it to use an R value instead of IJKand it should work for you.
If the A.G.E. controller is similar to the SM or SMX controllertry setting the quadrant crossing to 90 per blockand the IJK from Start Point to center distance signed.
Also set the tape file extension to be gcd. Using a gcd extension tells the controller to use a g-code file.With most otherfile extensions the controller tries to convert the file to its internal program language. This may be whatis causingthe problem.
The Prototrak has been down for the count, but it's back up and running. What an antique this machine is!! I got the machine to communicate with ProE somewhat. I still don't trust it. Southwestern Industries said I can communicate G/M codes using .dnc. This where this "T" buisness happens. Maybe it's the 25 year gap between ProE and the Prototrak machine
For some reason it does not want to machine the letter "T" it will machine it a lower case "t" instead. What the heck would cause this?
Hi Tesla,
I copied the program into Predator and ran a simulation. I don't see what the problem is, it makes 4 passes across the top of the "T", 5/16" long, and 4 passes along the vertical leg of the "T", 1/2" long.
There are a couple of things I'm not sure that's needed or might be causing a problem. Try removing these.
1. The space after the N100.
2. The M06 at the end of N105.
3. The space after N370.
4. and the space after N375.
5. Try removing the G43 and G49 also.
Another couple of questions. When you say it does a lower case "t" instead. Do you mean with the code as written? I haven't had a chance to look at the post yet.
ProE creates the proper toolpath but the ProtoTrak gets messed up for some reason. It is only when a "T" is used as the first letter. ProtoTrak will change a "T" into a "t". I am using Iso-font and I tried using norm-font. It will do the same thing.
I noticed the the post has the box checked forX,Y,Z to be in the same line. Shouldn't this be checked so Z has it's own line move and then follow with X,Y next?
Hi Tesla,
I would say Yes to your question of having Z on separate line, IF you're talking about a rapid move. If this checkbox pertains to a linear interpolation or circular motion then you want the ability to move all three axes simultaneously.
The post is outputting the rapid movements on separate lines now by what you've posted.
Maybe we need to look at what is coming before this tool or is this the only tool in the program?
The next resolution is a bonehead suggestion - Program an additional letter at the beginning and delete it until you figure out the problem. I know I know - that's idiotic.
Do you have a manual for this control? Maybe it's some code that's throwing it into lowercase mode. That's all I have right now.
The PROTOTRAK usesthese extentions to run programs DNC, MX3 and CAM.
DNC__G and M code
CAM__Traslates G and M code into Conversational programming
MX3__Conversational program at the machine
The problems are coming from the Prototrak AGE 3 controller translating wrong. I thought DNC would be the best bet to run programs so the memory doesn't get full and I could run larger programs. But the AGE 3 controller has problems transfering the M and G codes. This is why the "T" was not machining proper. I saved the same exact program as CAM and it worked great.
I am still having problems when I try to cut araindow shaped part. Or bottle shape where I am using 2-axis simultaniously. This is a 2 1/2 axis machine not a full 3-axis. So I can only use X/Z or Y/Z simulataniously. We inherited this machine fromone of ourfacilities that was closed down. It is pretty limited of what it can do.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
