Pro/NC Sheet Metal Opinion

[vandewinckel]

We're using SmartCam and we are thinking of switching to Pro/NC for Sheet Metal.


We are currently using Pro-e Wildfire 2.0 for modeling


Is there anyone out there using Pro/NC for sheet metal.


I'm looking for opinions on the user interface, auto nesting, reliability of the softwareand pretty much anything else to do with Pro/NC Sheet Metal.


Thanks Steve

 

[marker4x4]

We're using SmartCam and we are thinking of switching to Pro/NC for Sheet Metal.


We are currently using Pro-e Wildfire 2.0 for modeling


Is there anyone out there using Pro/NC for sheet metal.


I'm looking for opinions on the user interface, auto nesting, reliability of the softwareand pretty much anything else to do with Pro/NC Sheet Metal.


Thanks Steve

I used ProSheet a while ago (2000i2) and it's been pretty good. I would imagine that WF2 is even better

In any case, SmartCam being a really old and inefficient system is nowhere near WF in any aspect, whether modeling or NC.

 

[vandewinckel]

Mark


Thanks for the response


Steve

 

[conrat]

I have only used two programs for sheet metal punching. One was
JetCAM, which is really hard to use. The other is NC/Sheetmetal
for Pro/E. Pro/E's NC module is nice. It is a bit quirky
though and has not been updated since at least release 2001. It
looks and bhaves exactly the same in 2001 as in WF3. Dashboard
functionality has not been added. It also has a tendency to load
tools into stations that do not exist on our punch press.



For instance, we have a 36 station punch press, but if I choose a tool
that is not in the turret, instead of asking me to replace another
station, it sinmply adds station 37, even though the setup params tell
it there are only 36 stations.



Also, it likes to index dies, even when you set up the tool as a
non-indexing station. This obviously can cause problems, as the
tooling looks correct.



Just some thoughts. If Smartcam is working for you, you might
want to look around before plunking down the money for NC/Sheet Metal.



Jim

 

[vandewinckel]

Thanks Jim that exactly the kind of information i'm looking for.


Steve

 

[indigo2]

Steve -
There is an easy answer to both of these items.

First is the automatic addition of "station 37" that Jim (Conrat) mentioned. In the parameters definition section of the workcell, there is a parameter, AUTO_EXIST_TOOL_ONLY. That should be set to 'yes', to dis-allow Pro/E from creating a new station if it is needed. The downside to that is that if you use auto punching, and there is no matching tool available in the turret, you will not get a hole punched. (unless, of course you set it up manually)

Second is the issue of Indexing. Again, the UI provides an easy answer. From the Turret manager window (also in the workcell), there is a checkbox near the bottom called "Indexability". If that is checked (the default setting, btw) Pro/E assumes that the tool _is_ indexable. To change that, simply un-check that option. Additionally, specific angle can be defined in the "Orientation" box, just to the right of the Indexability item.

Hope that helps. As I mentioned earlier, I am more than happy to take a live call on this if you are interested. I can probably answer most any question regarding NC-Sheetmetal.
Have a good one!
-tsl

 

[conrat]

tsl,



Thanks for the AUTO_EXIST_TOOL_ONLY option.



Do you know what the parameter MAX_TURRET_SIZE does? I thought this
was where you set the maximum size of the turret as in number of
stations. If this is what that parameter is for, then Pro/NC
completely ignores the setting, as it will add stations above and
beyond the setting of this.



The indexibility check box does not always work as you mention. I
have a 1/4" x 4-1/4" rectangular die that I place in a station at 0
degree orientation and tell Pro that the station is not indexed.
We also have the same die in another station set to 90 degrees, also
not indexed.



Pro/E (as of WF3 M020) will automatically index the wrong tool, instead
of using the one I have oriented correctly. This is a
reproducible problem that happens everytime we try to use the 90 degree
station.



I will continue to look into this, using your suggestions.



I probably have a million questions for you on NC/SheetMetal. I will let you know how I fare.



Thanks for your help.

Jim

 

[indigo2]

Jim -
I'd tend to agree with your observation on MAX_TURRET_SIZE being broken. I have not implemented that, but I tested it after your reply. It seem to be ignored...

On the Indexability, I think that NC-Sheetmetal might be using another tool to punch the rotated hits. I just looked back at a model I did a while back, and I had the same slitting tool loaded in 2 stations, one at 0, the other at 90 degree. The sequence cut all the way around the part, but it used both tools, and did not index either one. You might check the ncl code to see if another tool is being called out, rather than indexing the first one.

I also had a couple of notches that would require the (same slitting) tool to index some odd angle to complete the perimeter cut on the part. With the tool set to non-indexable, those notched cut were omitted.

One other parameter that you may find helpful is

NE_LOCKED_TOOL_ORIENT. That can be set to an angular value (like 0, or 90 degrees...) so that the tool only punches with the long edge running parallel to the value you entered. Kind of klunky, but it does force the issue.

HIH...
-tsl

 

[conrat]

Thanks. This information should prove useful. I will try some of these settings and see what happens.



On another note, do you know an easy way of determining overall flat
sheet size (we call it girth here at the factory). This would be
the total unfolded length of the part.



The way I have been doing it is creating an UNBENDALL, then using an
evaluate feature to dimension from the edge of the part to the other
edge, setting the resultant value to a parameter, then adding BENDBACK
all to the part.



It is quite a pain and I am wondering if there is an easier way. Maybe an internal parameter or a better method.



Thanks,

Jim