Need Help!- ProE Wildfire 3 Manufacturing Questions

[Joe_Public]

Guys,

I'm trying to get to grips with Wildfire 3 Manufacturing - ie getting gcodes out for use with Mach3 controlling a 3-axis cnc mill. A few questions:

1) When Volume milling, and playing the toolpath, how do I display the 'in process' geometry? For examply, how can I show the removed material in real time when playing the toopath? As I've got it at the moment, the path CL is displayed, but I can't easily visualise what the machined part looks like. BTW I don't have vericut.

2) How do I get the approach angle of the end mill right? I need to specify an angle at which the mill will initially graze the surface - which dialogue box is this input in?

3) Is there a specific post processor to get from Wildfire 3 into Mach 3 without messing about editing?

Cheers in advance,

Garth.

[Joe_Public]

I take it from the total lack of comments that ProE Wildfire isn't the best software for this kind of thing!

[JonasC]

Hej Joe,

quite the contrary, it's the best program for just about everything (CAM related at least)
Just havent been in here for a while.

1. When you choose 'Play Path' from within the NC Sequence, you'll get the options for 'Screen Play', 'NC Check', and 'Gouge Check'.
They do:

'Screen play' - This seems to be what you currently use. Simply displays the toolpaths without Material removal. Great way to fast and easy see the general appearence of it. You can position the tool throughout the toolpath and measure clearences etc.

'NC Check' - This would be what you look for. Performs a material removal simulation where you actually see the workpiece being machined. You claim to not have Vericut? There's always(since like release 200i2) a basic vericut version shipped with ProE thats installed. So most probably you DO have vericut installed only not the full version.
However, should you really not have it or wanna try ProE's older native (and nowadays unsupported) material removal simulation, simply go to 'Tools' / 'Options' and set the 'nccheck_type' parameter to nccheck.

'Gouge check' - simply checks if tool gouges the part throughout the toolpath. Can ofc be done in the material removal simulation but this is just an alt way to get a quick indication.

Now, should you want to simulate your entire operation, you need to output it to disk first, Do this by (from topmenu) 'CL Data' / 'Output' / 'Operation' / Chose your op / 'File' / 'Done'. The to simulate it: 'CL Data' / 'NC Check'... from there on it looks different depending on your option is set to NCCHECK or VERICUT, but I guess you'll manage from there.

2. The angle of attack is specified in the NC Sequence parameters. You'll find it near the bottom and it's called 'Ramp_angle'.

3. I think I've seen some floating around, maybe there was some info on the mach3 homepage. Check there to start with. If I remember correctly the mach3 is pretty similar to fanuc iso right? Then you might be good to go with one of PTC's standard postprocessors. If you have active maintenance you can download them from ptc.com.

Good luck and let me know if there's something thats still unclear.

/J

[bartL]

Joe,

I'm using Pro/mfg in combination with mach 3 too. I control my Bridgeport series 1 with it. I don't know if you have the standard postprocessors in you MFg application? I always use the first post processor, that one works great on my machine. Beside that I think your mach3 setup has to correct too.

When I've made my toolpaths I can simply press a simple mapkey code and the complete G-code of the operation has been saved on my disc
Although I think Pro/Mfg has a steep learning curve and very difficult to learn if you don't have Pro/e experience.

Bart

[Joe_Public]

JonasC,

Great information, thanks!

When I select NCCheck, I get the message

"Application VERICUT_DLL is not available or supported on this platform."

So, as you suggested I went to Options and found the NCCHECK option, which loads fine and appears to work. I saved a new cutting file and then went back and selected NCCheck in the menu, and ran it, but it now just plays the tool over the *finished* geometry (in a rather fetching shade of purple I might add), so still no real time cutting view. Also, there appears to be no way of stopping, slowing or speeding the animated path. Any ideas? I've created a volume mill, (where I subtracted an extruded rectangle of material from the required finished geometry in order to create a selectable geometry block of the removed metal). Toolpath plays great and everything seems ok apart from this real time volume removal issue.

Thanks again for your suggestions!

Bart,

I've been using ProE for design and assembly work and Mechanica for stress analysis for about 10 years now (since I think release 18) as a designer of offshore castings and currently aerospace components. The manufacturing option is a bit of a hobby for me, in that I want to eventually build a CNC mill, but I want to be sure I can tackle the CAM side of things first before investing hard earned cash into a stepper controller and motors etc etc. I have used an in-house translator at work which I've got working with Mach 3 (output for a "MakinoA995XR" !? seems to work fine), but I will try the standard outputs as you suggest. I always seem to take the most complicated option first!

Cheers,

Garth.

[bartL]

Joe,

Once you've made a toolpath just go to output, operation, file and select NCL. There you can name the file, once you do this correctly, it will take you to the post processor automatically. Just select the first one in this row and it works fine with mach3. No machine name or type of control have to be selected there. I don't know where exactly you're selecting the PP? I can remember I found some machine types somewhere to when I tried to find out how to post process the file but that seemed to be the wrong way for me.
About mechanica, the company I work for has decided to buy some mechanica licences and I think I have to learn this to. Now I'm working with ANSYS for a very short while, do you have any experience with this program? And do you have any experience with fatigue strength calculations on welding assemblies?

Thanks,
Bart

[JonasC]

Hej Joe,

Seems strange. It's like you don't have a workpiece defined. Which you do have right?
Have you used any Material Removal features?
Would you consider sending me the files, or something else(an example) if your stuff is a bit secret?

Attached a few screenshots of NCCheck vs Vericut for your consideration.
Basically Vericut is better in all aspects; dynamic sppedcontrol throuhout the simulation, dynamic reorientation throughout the simulaton, better resolution and a whole bunch of other features.
NCCHeck though can sometimes be used when you wanna check something a bit quicker. I tend to switch between them, maybe using NCCHeck more when defining my sequences and then final checks in Vericut.

Since you obviously don't have Vericut installed, I think someone made a conscious choice not to install it, since it is shipped on the same CD as ProE and preselected to be installed. Check with your IT dep.


Piece to be cut


NCCheck


Vericut

BR, Jonas

[JonasC]

eeerh, come to think of it I'm not really a 100% certain that Vericut is default to be installed when installing ProE. Check that under options when installing, I.e. run ptcsetup.bat. Let me know if you have problems checking that.

Also I know there was some issue with WF3 datecode M090, so if you have that datecode let me know and I'll check the remedy.

/J

[Joe_Public]

Originally Posted by bartL Joe, Once you've made a toolpath just go to output, operation, file and select NCL. There you can name the file, once you do this correctly, it will take you to the post processor automatically. Just select the first one in this row and it works fine with mach3. No machine name or type of control have to be selected there. I don't know where exactly you're selecting the PP? I can remember I found some machine types somewhere to when I tried to find out how to post process the file but that seemed to be the wrong way for me. About mechanica, the company I work for has decided to buy some mechanica licences and I think I have to learn this to. Now I'm working with ANSYS for a very short while, do you have any experience with this program? And do you have any experience with fatigue strength calculations on welding assemblies? Thanks, Bart

Bart,

OK I'll try to use the PP as you describe.

I don't have any experience of ANSYS, sorry.

My experience of Mechanica is almost 100% Linear Static stress analysis of large castings. I don't have much experience of welded assemblies. What we used to do was model a casting, then add the incoming plate members onto it, load the ends of the incoming members and see what the peak stresses were at the weld interfaces. When youre welding a plate to a casting you usually have a tapered region of casting which finishes at around the width of the incoming member (to avoid any 90 degree corners). Even then you end up with a slight discontinuity at the weld plane which can give an unrealistic very high peak stress in that region, so we sometimes had to use an 'equivalent weld plane stress' which was obtained by drawing a graph of stress vs distance from weld interface; the technique was to extrapolate the shallow part of the graph gradient (from defined distances away from the weld plane) back to the weld plane axis (usually x=0), thus cutting out the sharp peak.

The vast majority of my work was solid models of both casting and plate, rather than shell models (commonly used in fabrication items) and I know that if you try to model thin plate in solids and load it, you will tend to get massive peak stresses in the corner regions, which might make fatigue analysis tricky. Perhaps there is some way of avoiding this in another ProE package? Perhaps someone else with direct experience could help you here?

I'd assume that what you're wanting to do is model the assembly, load it and obtain peak stresses from the FEA so that you could then plug into another application or even just a fatigue equation to get a fatigue life?

Sorry I can't be of more help.

Regards,

Garth.

[Joe_Public]

Originally Posted by JonasC Hej Joe, Seems strange. It's like you don't have a workpiece defined. Which you do have right? Have you used any Material Removal features? Would you consider sending me the files, or something else(an example) if your stuff is a bit secret? Attached a few screenshots of NCCheck vs Vericut for your consideration. Basically Vericut is better in all aspects; dynamic sppedcontrol throuhout the simulation, dynamic reorientation throughout the simulaton, better resolution and a whole bunch of other features. NCCHeck though can sometimes be used when you wanna check something a bit quicker. I tend to switch between them, maybe using NCCHeck more when defining my sequences and then final checks in Vericut. Since you obviously don't have Vericut installed, I think someone made a conscious choice not to install it, since it is shipped on the same CD as ProE and preselected to be installed. Check with your IT dep. [BR, Jonas

Jonas,

The date code is M030.

The images you posted are exactly what I'm after, but still no luck. I am using 'Mill Volume', no Material Removal Features. All I did was create the finished geometry (see attached "Finished_Geometry.pdf"), then, within 'manufacturing' I created the volume of material I wanted to remove, and selected this when prompted "Select previously defined milling volume". I can play the tool path (see attached "Toolpath_Wireframe.pdf), and if I shade this view, you can see the volume to be machined away is definitely there (see attached "Toolpath_within_shaded_volume.pdf"). When I followed your initial instructions for NCCheck, I get a toolpath played over the geometry in "Finished_Geometry.pdf", which isn't much use!

I'd rather not send files (even though it's just a sign for a house!), but thanks for the offer of help.

I ran ptcsetup.bat, but, at least on the screen that comes up initially, Vericut is not there.

Thanks for your help,

Regards,

Garth.

[JonasC]

Joe,

Lets just try with a Pro/NC file of mine.
Just run NCCheck on one of the sequences and let me know if it looks allright.

pwd in pm,

/Jonas

[JonasC]

Where to find the Vericut install option.
Note that you need to install from CD to get it installed. Running ptcsetup.bat will only show you that it is not installed right now.

/Jonas