[pinguS]

Hi

I think this is the right operation, but I'm getting stuck right at the beginning. I know this must be simple but if I just have a solid piece of material, say 6" square or round. I want to be able to just profile a shape down.

More explaination:
The thing Im trying to make looks a pair of bonoculars, sort of, i.e. a 50mm diamter circle in the middle 80mm depth. Connected to this are 2 stems either side half way down, but these are only 20mm, square. And on the ends of these are 2 circles 30mm diameter also only 20mm depth (so these are in located exactly 40mm down centre to centre)

When I select profile, if I need to just mill the external shape down, I imagine you have to use "Curve and Auto-constant Z" to define the profile, but where the stems connect to the main circle, being half way down, it doesn't have any lines to select, only a face, which then alarms "Chain must be continuous"

I have a 80mm depth by 6" billet clamped down (6" round). All I'm need to do is profile the outer shape out, the rest I can hopefully manage to set up in Solidcam. The part is solidworks.

So was wondering how the heck do I mill a shape out, just external shape if I can't select lines?

Does this make any sense at all?? I have attached a picture of what I'm making

[Brakeman Bob]

There are various ways of tackling this. One is to go to the feature tree in SW, right click on CAM part and select "Edit Part". Then select the top face of the part, right click and select "Insert Sketch". Once in the sketch select the edges you want to form the profile and convert the entities to sketch lines. Stop editing the sketch, go to you SolidCAM job and define the profile from the sketch you've just created. Voilá.

Another way is to open up the CAM part for editing, select (or create) the plane which bisects the part at a place where the profile is as you want it and ceate a sketch. Then via sketch tools selrct "Intersection Curve" and pick the faces of the profile. Then define the geometry as before.

The CAM part is a very powerful tool in defining geometry and opens up all the usability of SolidWorks for controlling the tool path. For example, setting up a work area or constraint boundary, offsetting a face and filling it to act as a mask in 3D machining. I'd be lost without it.

[pinguS]

....The CAM part is a very powerful tool in defining geometry and opens up all the usability of SolidWorks for controlling the tool path. For example, setting up a work area or constraint boundary, offsetting a face and filling it to act as a mask in 3D machining. I'd be lost without it. ....

Can you explain more on this, or when you say open up the cam part, do you mean actually open a file in solidworks which has been created in solidcam??

Brakeman, I really hope Solidcam have given you excessive shares in their business, assuming you are not linked to them, as I don't actually know where they would be without you.....

[pinguS]

Ok that worked, using a profile line created in solidworks, which has led me to another problem I though would be easily solved, but I'm struggling....

If you look at the 2 circle lugs to either side of the big circle, I thought I obviously need to use a face mill operation to bring them down to the right height (currently still has stock material to machine off), but using this it cuts straight through the big circle, not around it. I have even tried by separating each face when defining the contours.

Should I be creating seperate operations for each side circle, instead of trying in one operation? Or am I just using the wrong operation.

I have tried profile again, but it just doesnm't calculate anything (nothing showing in the simulation...)

hmmmmmm

[pinguS]

Ok another thing I have just tried, or tried to do was change the direction of the face operation, but I can't seem to get it to go back and forth in Y axis direction, it only seems to go in X axis back and forth...

..........Ok worked this out, this is the angle setting in data setting for Hatch on face operation.... but still struggling to machine down the side circles

[Brakeman Bob]

....The CAM part is a very powerful tool in defining geometry.....Can you explain more on this, or when you say open up the cam part, do you mean actually open a file in solidworks which has been created in solidcam??

Brakeman, I really hope Solidcam have given you excessive shares in their business, assuming you are not linked to them, as I don't actually know where they would be without you.....

When you are working in SolidCAM, the Solidworks window is showing and assembly - your part is named "Widget.SLDASM" - and looking in the SolidWorks Feature Tree shows at least two parts

"DesignPart" - this is the clone of the part you are programming code for. SolidCAM creates the clone so that nothing untoward happens to your original and for speed purposes. This clone is associated with the original and if the designer changes the original model SolidCAM will rpompt you to decide if you want to update tour "DesignPart". Do not mess with the DesignPart as it can have odd outcomes if the original is changed.

The other part is the "CAM Part". This is an empty part created by SolidCAM for you to do your stuff in (if you put sketches etc. in at the assembly level it don't half slow down processing if you have a big part and lots of sketches). This part is associated with the "DesignPart" and therefore if say you create a sketch using entities in the DesignPart which change, your sketch will change. You can do anything you like in the "CAM Part" - it is what it is there for.

Of course there is nothing stopping you from adding to the assembly - I have all our fixtures modelled, so I add them in order to do collision checking. I also add the billet or forging from which the part is machined and then use this model to define my stock.

I don't have shares in SolidCAM - I am just a (relatively) happy user who like to pass his knowledge on. I think sometimes that SolidCAM get a little fed up with me as I do seem to find bugs that no-one else reports, but I put that down to the complexity of our parts and my determination to stretch the software.

[Brakeman Bob]

Ok another thing I have just tried, or tried to do was change the direction of the face operation, but I can't seem to get it to go back and forth in Y axis direction, it only seems to go in X axis back and forth...

..........Ok worked this out, this is the angle setting in data setting for Hatch on face operation.... but still struggling to machine down the side circles

If you have defined your billet you could use the outer edges for a profile job to machine the side circles. Go to the Technology tab and click on "Geometry" to extend or offset the lines. Alternatively sketch a horseshoe shap in CAM Part and use that in a Profile job. The cutter path doesn't have to be linked directly to the part geometry.

[pinguS]

I didn't actually think of that (horse shoe)

I was assuming use would just select the areas to machine and solidcam would pick up on the fact is was going to cut away at an undefined area of the part (the big circle), which would then change the final part when side circles are machined.

Can machining boundaries not be defined, i.e. tell solidcam it cannot cross the big circle profile when calculating machining of the small circles. Either way, i'm going to go with horse shoe style and see what I get...

[Brakeman Bob]

No CAM system I'm aware of is that smart. Delcam's PowerMIll comes close but it is amied more at the Mould & Die sector (at least it used to be).

[dengo]

If you have HSM you can also use the combined boundary option which will allow you to play around with the interaction of previously used boundaries to produce new ones.
But the best advice with SC is KISS......

[Brakeman Bob]

If you have HSM you can also use the combined boundary option which will allow you to play around with the interaction of previously used boundaries to produce new ones.
But the best advice with SC is KISS......

I've seen that combined boundary option and I believe that you can also do boolean operations with boundaries. Never have cause to use it yet but I am intrigued.

[pinguS]

What part of solidcam are you guys talking about, how do I check If I have the HSM options as this is not my company, and the owners are lets say not so clued up...

I would like to know more on this boundary option...

[mattpatt]

One of the best features (in my opinion) is the ease at which you can create boundaries, work areas, profiles etc so as to keep the tool where you want it, or just make some lines for the tool to follow.

Very often I'll make a plane in the CAM part and just sketch some geometry, or convert a few lines or what have you.

As with all the options HSM offers, I still haven't used them all! but I'm working at it.

[dengo]

What part of solidcam are you guys talking about, how do I check If I have the HSM options as this is not my company, and the owners are lets say not so clued up...

I would like to know more on this boundary option...

To see if you have HSM.
In your SC part go to add a new operation, another menu appears with the types of ops to choose from. The first group are 2.5D then the drilling & pocket module, next is surface machining then 3D ops etc etc etc. You should be able to see all of the modules listed but if they are greyed out its not available with your licence.
If its not your SC reseller should be able to give you a temp licence to try it out. that's what we did at first in here.

[dengo]

One of the best features (in my opinion) is the ease at which you can create boundaries, work areas, profiles etc so as to keep the tool where you want it, or just make some lines for the tool to follow.

Very often I'll make a plane in the CAM part and just sketch some geometry, or convert a few lines or what have you.

As with all the options HSM offers, I still haven't used them all! but I'm working at it.

HSM is no different than 2.5D or 3D when it comes to easily creating sketches or boundaries.
Where is does come into it's own is the software its self.
SC is years old and every year they add more features and try to fix old bugs ( like Bob pointed out in another post I also seem to find more than my fair share of these bugs.......)
The problem is that these additions and fixes (already SP3 for SC2009 which is less than 12 months old and SC2008 was worse needing up to SP4 before they gave up and released the next version) are built on the previous software engine. So these problems can reappear or morph into something else.
HSM was built from the ground up as a separate module. You can run HSM without 2.5 or 3D if you like. I just find it to be (relatively) more stable in comparison with 3D. It's not perfect but it's better

[Brakeman Bob]

HSM is a module licensed from another CAM software house that concentrates on Mould & Die. It was originally aimed at users who had older machines that didn't have the sophisticated Acc & Dec in their control that is required for true high speed machining. Compare the behavior of a tool when doing a bi-directional toolpath; 3D just reverses whilst HSM offers all sorts of control - the tool arcs off the part and loops through curves to change direction. However, 'taint honey 'n roses all the way. I still use 3D roughing because it gives better control over the tool approaches.

On the subject of unknown modules in SolidCAM, I'm still trying to think of a need to use the HSS module. Any ideas?

[mattpatt]

I find the 3D milling good, but sometimes I have issues with the tool plunging in to too much material etc. As you say Bob, with HSM I can control this and now use it a lot both roughing and finishing. However, in some cases I revert to the 3D milling (constant Z) as I seem to find it better for constant step over features on tapered walls. Maybe just something I'm not doing right in HSM.

Gave HSS a test. Made one part already using some HSS cutting, but now considering redoing it and using HSM. On another part, the only area that seems to benefit from HSS is a variable fillet running around the edge of the part, but as I haven't made it yet, I can't say how it'll come out. The tool path looks kind of interesting though with very little air time.

[dengo]

I was under the impression that HSM was built by SC but that the 5 Axis module is indeed a 3rd party add in.

HSS is just a stripped down 5 Axis operation converted for 3D machines, it uses the same basic engine and the user window looks very similar. Like most CAM systems there are many ways to skin a cat but again it seems to have a stable engine running the toolpaths and the Gouge Check is a very powerful control.

As for 3D v HSM... I have never felt the need to go back to 3D for any job I have done. We had the same issues on certain jobs of plunging into too much stock but I've not had any issues like that with HSM. It sounds like I use Constant Z much like you guys. For good control of step over, in the Passes area there is a tab for Adaptive Step Down. In here you can play around with the Profile Step In and Scallop controls. I find these useful for parts with variable taper.
When it comes to controlling approaches you can have as much or as little as you like. Set all of the approach ramp & extensions & curls & rads & angles and all the other options it gives you to 0 and Hey Presto you have 3D roughing but without the nasty surprises. I have a roughing template set to just that for certain jobs. Another good thing with using HSM is that all Rapid moves are replaced by high feeds instead. We've had several parts that got scrapped because the rapid move clipped an important feature even though SC thought it wouldn't. With a G01 instead of G00 I've never had that problem.
And at the risk of preaching to the choir Wall Draft Angle in 2.5D Profile Milling is good for using on a lot of tapers I deal with.
Sorry for the GIANT post

[Brakeman Bob]

I tested HSM before it was released and I know which CAM company they licensed it off.

The time I revert back to 'old' 3D is constant Z semi-finishing of a part roughly blocked out; I use the "Cut only rest material" option in Work Area and then set the approaches to normal or arc or whatever. I found that trying to do the same thing in HSM meant the tool plunged in on the blocked out part (though recently I discovered a setting that allowed you set the plunge point as a Drill geometry but I haven't used properly yet).

I suppose my trouble is I need to do as much 2½D machining as possible before moving over to 3D / 5X - our parts have reference surfaces that are used in later operations and these really need to be endmilled rather than scanned with a ballnose.

Need to change my mindset I suppose.

[dengo]

The time I revert back to 'old' 3D is constant Z semi-finishing of a part roughly blocked out; I use the "Cut only rest material" option in Work Area and then set the approaches to normal or arc or whatever. I found that trying to do the same thing in HSM meant the tool plunged in on the blocked out part (though recently I discovered a setting that allowed you set the plunge point as a Drill geometry but I haven't used properly yet).

You have the same level of control in HSM. It's in the Edit passes tab of a contour roughing op. Set stock surfaces to "Updated Stock" instead of "Main Geometry", you can then also use the "Overthickness" to adjust your toolpath. I use this for castings as opposed to billets of stock. But the actual Rest Roughing strategy is certainly the best I have used. You also have the same ability to limit the passes as before with stock overthickness.

I remember asking one of SC's guys a few years ago for advice with rest roughing in 3D. He said "Don't Bother". No problem with HSM though, very quick calculations and no messing around trying to control toolpaths with a semi finish Op.
Again though, there are so many ways to get to the same result in the end so it all just comes down to what works for you. We found that were all happier with HSM than we were with 3D (although there were huge temptations to go back while we were trying to get up to speed).