[cnckyle]

Just got the demo of Solidcam and rather like it so far.

I was curious if anyone knows how to load multiple parts on the screen and tell it to mill all of the pieces on 1 stock material piece.

Thanks. Oh yeah it is SolidCam2009 if it makes a difference.

[mattpatt]

Several ways to do this. Here's how I do it, but it all depends on your parts.

1) add configuration in SW model. This could just be a block or a half machined part. A couple of examples for me are when I make motorcycle triple clamps. When the design work for the part is done I add a configuration called "stock", then extrude a simple chunk of material over the part which is the 'real stock' I order. I then suppress this extrusion in the default configuration.

I also make a couple of parts that has some turning work before the CNC work. I use this semi machined model as the 'stock' configuration.

In Solidcam, at the first stage you can select configurations (either default or stock) as your target and stock.

2) Let SC build your stock. Again at set up you select the part as a box (auto) or something like that. Select your target and SC will build material round it (a box) with extra material that you need.

3) As above, but select multiple parts for one big block.

Hope this helps.

[Brakeman Bob]

To get multiple parts in your code (assuming your post processor has been set up correctly for procedures) is to select all the SolidCAM jobs, right click and go "Transform", then choose your option. I have mainly used it for the "Mirror" transform but there used to be options for shifting the code in X & Y (btw, before you get excited, the mirroring sucks).

I don't know if the transform features work in SolidVerify.

Bob

[mattpatt]

I use the transform / translate / Matrix quite a lot. Use for multiple parts on a jig, and if I'm using a pair of vices holding the same part.

Works well for me.

Also use the rotate / Delta option on a couple of jobs.

I had to play with the gpp file a little to get things working right, especially for the rotate. For this I added a couple of extra variables for the rotation angle, which are set by the operator from the main program.

They both work quite sweetly now, and solid verify will also show you the toolpaths. Although if using the Delta or Matrix options (which generate a loop in the program and moves the datum by increments) I don't get to see these toolpaths in CIMCO Edit V5. Maybe I have it set up wrong but it's not a big thing.

I had a problem if I was roughing a part, then using the same tool to finish but at a different speed (all within the same loop). First it didn't see this speed change but would then cut at the new (finish) feed. Got that sorted, and also put in a G4 x1.5 delay so that things would get up to speed before getting stuck in. Then when it got back to the top of the loop (and moved to the next position) it once more didn't change the spindle speed, but sorted that out with some more code in the gpp file.

It's a cool feature (transform) and saves a lot of file space.

Bob, I've not used the mirror feature, because when I had a play it reversed all the toolpaths. So climb milling became conventional etc. Sorry, but I'm not having that....not on my watch!

[Brakeman Bob]

I don't use the mirror feature for that very reason. SolidCAM were developing an automatic mirroring function that kept the cutting direction a couple of years ago (I tested it) but then they lost interest. Now I see that OpenMind offer a mirror function that keeps the direction of cut (allegedly) in their latest incarnation of HyperMill. I shall be checking that out when I get time.

[dengo]

Transform, Translate , matrix is the way to go. The problem with Mirror is that if your Part is Handed in any way then you'll get the opposite hand of that part. If that is what you need then I'd mirror the part in SW first and set my job to machine both parts together.
The same goes for doing several different parts but using the same stock. Set everything out in SW as an assembly stock and all, then start a new SC part from that assy.

I'm in a prototype dept of a large organisation & I've been using SW/SC for 4 years now and I find it best to do as much preparation as you can in SW first.

[mattpatt]

I agree with mirroring a part in SW before starting the cam, but I have to say that usually I use transform, translate, matrix when doing several of the same parts. Keeps my program nice and neat.

[dengo]

Definitely if you are making multiples of identical parts. It's a great feature

I often have to make prototypes of the same part but with certain features having a variation of sizes or even several separate parts from single stock if I want to run overnight. In that case then transform won't work.

[cnckyle]

Thanks for the responses. I will try what you guys suggest this weekend.

[Brakeman Bob]

I invariably make mirrored parts in SolidWorks. My workflow goes as follows

Recieve part from Design - normally the LH part
Make CAM program
Do a "Save As" with CAM program giving it an appropriate name (say "RH_PART")
Make a mirrored part of the original Design model
Change the model reference in RH_PART to the mirrored part model
Reset all the MAC positions (this can take some time - I've found it useful to generate sketches of geometry just to get the definition of the MAC and then mess with the 3D sketch that defines the MAC to change the direction).
Mirror the sketches in CAM part
Redefine any dangling geometry.