Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

prototyping in pro manufacturing

C

cncwhiz

New member
I work for a small "50 people" company. We are working on some new products. The highups are looking for my process to be streamlined. We are a production shop so we are setup to run "batch" machining. I have an area that I keep tooling seperate from production for doing prototype. I am building a selection of tools, drills, taps, endmills for this purpose. What I am looking for is a better process to get the part off the machine where we can set a time frame from the begining of planning to the part comming off of the machine. I their eyes, the time to do this process is too long. We do alot of deep hole drilling, tapping and threadmilling. I am also the guy that has to do the job at the machine. I just built a job with over 40 tools. Any ideas other that the painstaking tool by tool line by line prove out? I am looking for any input in this mannor..
 
I have been doing some hunting for ideas on dealing with most of these issues. First off, it seems to me that to simulate or varify a milling sequence most cam softwares are addressing this issue. Vericut imbeded software in proman also address this issue. Most people doing hole drilling don't need the depth to be close so .010 here or there is not an issue. In manufacturing hydraulic valving this issue is very important as that shallow depths cause flow restrictions and deep holes cause problems with turbulence issues.It seems like this issue can be addressed but I need to have a data base of my drills with the correct "tip offset". Thiscan be a problem in that depending on who manufactures the tool drill point angle and a flat on the end of the drill change. Most of my holes are drilled with parabolic drills with a 130' point. To build this database will be a PIA. Theother way to deal with this issue is to purchase a seat of vericutwith "autodif" option. This will allow the process to be done using the gcode and tool model and check the material removal for excess or not enough stock removed. The other issue is with tapping. In the tool parameters you can set the chamfer lengths toget the correct depth. This can and will work for "rigid" tapping. I have some older machines that use tension and comperssion tapping. This changes the ball game for the chamfer length in the tool parameters. The amount of travel depth varies from machine to machine in this style of tapping. This issue I think will have to be addressed in my post. The post will have to have a offset amount by machine to compensate for this difference.PTC has some things that they need to get on the ball and fix. Cosmetic threads are a joke! How can they do all the complex things they do and not be able to even do a thread that can be seen in manufacturing? The other thing that sucks as well are pipe threads. I have to build asweep and put a datum curve to machine apipe thread with a thread mill.
 
CNC,


I feel your pain with this. Unfortunately, with your drilling/tapping process (minus the compression/tension problem) being so demanding, you are really going to have no choice except to accurately define/describe the tools you are using in ProE. This means also specifying the exact manufacturer, etc, and having a way to make certain that the shop adheres to the specification. Auto-Diff is a great Vericut feature, but it is only going to show you what you already know. If the drill in the Tool Manager doesn't exactly match the tool in the spindle, you are going to have problems.


Regarding cosmetic threads, I am not experiencing the problems that you are with them. I can see them well enough and can determine visually if the tap is going to the correct depth. Having a swept cut would cause a massive performance hit, and I don't know of any other CAD program that does it differently as a matter of course.


Finally, we also do a lot of single point thread milling of pipe threads. We have a small library of UDF's for each thread size, and just add this UDF of the helical curve to the part where needed and then put the trajectory sequence on it. I actually find it easier to do pipe threads than straight threads in Pro/NC this way.


Regards
 
peterbrown77 said:
.... Finally, we also do a lot of single point thread milling of pipe threads. We have a small library of UDF's for each thread size, and just add this UDF of the helical curve to the part where needed and then put the trajectory sequence on it. I actually find it easier to do pipe threads than straight threads in Pro/NC this way.
Click to expand...



I don't mean to hijack this thread, but Peter - I found your threading method very interesting; would you mind sharing your UDF's with us?? Same as CNCwiz, I don't like the way ProMan does thread milling at all and would love to be able to use different way to do that.



Thanks,

Edited by: marker4x4
 
Having trouble putting them on the site; might be a firewall problem on my end. Someone else want to give it a shot? I was putting them in the UDF/Piping section.
 
peterbrown77 said:
Having trouble putting them on the site; might be a firewall problem on my end. Someone else want to give it a shot? I was putting them in the UDF/Piping section.
Click to expand...

I can try... perhaps you can email it to me and I'll post it up. My email is
mark at metalaction dot ca

Thanks!
 
Does your CNC control have subprograms like Macro "B" is a Fanuc control.





If you write sub programs they will give very predictable results and reduce


your prove-out time considerably.
 
I have a custom post that builds sub routines outside of pro. I run six sided tombstones for my production. I run the same parts on all sides so all I have to do is program one part and it subs and rotates automatically. I have been talking with Peter on this issue and the only way to do this correctly at least at this point for drilling is to model all of my tools and when I do a drilling sequence do a "blind sholder". When you set the hole depth pick the to surface and the do a "make datum" and pick the arc of the full diameter before the start of the tip. I think this method should work for taps as well. With the tapping the tap must have the lead built into the tool and then pick "blind sholder". The thing that I don't like about tapping is that you have to type in a number and it will not update with a rev?
 
The thing that I don't like about tapping is that you have to type in a number and it will not update with a rev?





I don't understand your problem.


As for the subroutine, instead of calling the sub we do a "Copy CL". Makes for a longer .tap file, but who cares?


Regards
 
I have a custom post that builds sub routines outside of pro. I run six sided tombstones for my production. I run the same parts on all sides so all I have to do is program one part and it subs and rotates automatically





I too have been going this way...it just makes life easier


I wrote it in VB and it takes the single .tap file and you choose how many you want and it does the rest...creates a .tap file with themulti name ..adds in block deletes..so I prove one..then toggle the block delete at the machine and run them all... I even have it spit out a setup sheet with a picture and means to upload to machine.....instr function in VB..so easy to get exactly what you want


as far as your present problem.... with the difference between machines...well sounds like your between a rock and a hard spot...


still beats tapping by hand tho
smiley2.gif
 
Peter,


What happins when the "model" has a revision and the thread depth changes? Blind with a plugged in depth does not update to be re-posted? As far as spitting out the cl, most of my programs have over 10,000 lines of code when they are built with a subroutine.


Wsylvester,


I am working with my post builder. He will give me a drop down when I post to the machine and I can plug in a variable for the difference between the absolute tap depth and the floating tap depth.
 
CNC,


If you do a "Make Datum" through the edge that denotes the end of the cosmetic thread for the 'end surface' in "Blind", the tap depth will be parametric to the part.





Regards
 
DUH,


Once again you have to slap me in the face to see the obvious. Make all the sence in the world! I am working on a program this afternoon and I will try it. Thanks Peter, again. Don't know if I will be able to see this afternoon thou. I have been going over 8,100 lines of code in my editor.


smiley32.gif
 
CNC,


That being said, I don't think you have to do a "Make Datum" through the end of the cosmetic thread - Pro is generally pretty good at driving the full diameter of the tap to the end of the cosmetic thread all by itself. What this means though, is that your chamfer definition on the tap has to be accurate to the actual tap.


Sorry to hear that you are eyeballing G-code. That is one task that Vericut Machine Simulation will relieve you of doing. It also pays to have a 'perfect postprocessor' in which you can have confidence that there are no surprises awaiting you on the machine.


Regards
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top