contain area will not work in solidworks CAM. disables the associated operation

I don't see a separate solidworks CAM forum but I think it is camworks renamed I'm new to solidworks CAM. I'm trying to clean up some material in some raised lettering inside a pocket bottom with a tiny end mill. For some reason the tool path generated does what I need but ALSO machines segments of the inside perimeter of the pocket, which has already been finish machined with a large end mill. The small endmill would take forever if I left that part of the tool path in. I used the contain functionality to try to keep the tool path where its needed, but no matter what I do or what setting I change using a contain area, that operation gets skipped. In the operations parameters I have under roughing tab rest machining from WIP, generate is checked. I have tried window and profile contain, drawn a sketch of the contain area and tried to use that, tried every permutation of settings that I was able to, all result in skipping the clean up operation I need. In other operations the contain function worked fine. I even deleted the operation and redid it, with no luck there either. What am I doing wrong? I don't know that I can use an "avoid" area because I need to avoid the interior perimeter of a pocket so I would need a donut shaped avoid area and I don't think there is a way to do that...if I pick the top edge or surface of the pocket to "avoid" it fills inward, no way to get it to make a donut..This is killing me.

What kind of operation are you using to do the final cleanup? Any chance you can attach the file in question, or at least a screenshot including the CAMWorks operation tree? You can PM me if its too sensitive to post here for all to see. It may be a matter of using the wrong type of operation for what you're actually trying to do, or it could be something as simple as having WIP machining or gouge checking turned on. I've been in this situation probably hundreds of times with CAMWorks and can usually find a way out of it!

Part of my problem is not knowing what I'm doing, I do a lot of CAD but very little CAM... I think I tried it with and without wip..I did reorder some operations to minimize tool changes. I also unchecked some boxes as this material does not need top cleanup or facing. I do have one "unable to offset one or more sketch entities" on the text extrude, but I was not able to find any error and the model looks perfectly fine, extruded properly, and I cleaned up some too tight areas. The operation to clear material with smaller mills in the same area works fine but there are some very small areas I need the 1/16 mill for. I just need to restrict the operation to cleaning out the text. I'm proving out a centroid router retrofit and wanted a relatively complex job to run on it...
thanks
tom

If it were me, I would program each letter segment as a boss with a fine or finish strategy. Generate all of those features once you have them all added, get the first one the way you want it (feeds, speeds, rapids, etc) then link the rest of them (right click first one>link operation) to "copy" what the first one does to all the other ones.

The problem with using a roughing strategy is that it is looking for areas where there is stock left over from previous operations and doing anything it can to try to remove it, within the guidelines of your strategy. There may be a way, with enough tinkering, to get it to do it but it is technically the wrong way. Try what I suggested above to see if it works for you. You can still PM me the file if you want me to take a look.

The thing that gets me is if the confine function worked properly I would be OK. I'm of course using too much of the automatic programming functionality and it works for the most part but.... I'll try a redo letter by letter

Its pretty quick if you do it right.

When adding the boss feature, just select the top of every letter segment at the same time and create them all at once.
After generating all of the operations, just focus on getting the first one set up properly.
After the first operation is done, use the "Link Operations" functionality to make them all the same.
There are a few things that don't copy over when using link operations, like individual leadins, so you may need to fix a few things manually but this method is pretty fast.

Note: you can link them all first then program the first one how you want it, but it will regenerate every operation every time you make a change so it can take more time if your computer is slow.

I ended up doing it all manually, much more concise then letting the automated system do it. Now I have another simple question- I had this solved last night but the above problem was so exasperating that I forgot - I have a sketch of a simple stick font on the same model that I need to engrave, but the sketch does not show up in the list of available sketches for 2.5 axis operations. how do I select it so I can do the engrave operation?

If its the "5536" text, I would use an engrave feature and that sketch should show up, unless there is something wrong with it like an overlapping line or something. Let me know if it doesn't work for you.

I got it; but I don't know why engrave doesn't show up in the initial drop down menu for 2.5 axis operation insertion, and you can't pick the stick font sketch as an available sketch unless you wade thru the menus to find engrave...not very user friendly...

Hmm, you should always have engrave as an option under any 2.5 axis feature insertion. I use CAMBAM stick fonts quite often for this type of application. They have a decent number of fonts and they seem to work well with most CAM software. While they are labeled as stick fonts, they actually are not because the loop back on themselves to create a closed loop. Do be able to be used in applications like solidworks, this is a requirement. That means that the toolpath will "double back" on itself during engraving. I haven't found it to be enough of a bother to mess with it, but on a really high volume run of parts you can always explode the text and delete the extra lines to shorten the cut time.

Your "2.5 Axis Feature..." dialog doesn't look like this?
https://i.ibb.co/QdtqfCs/CW1.png

No actually it looks like the attached, with the only choices being rough contour face or thread mill. I started by clicking on new 2.5 axis mill operation in the second down from the top tool bar. I'm still not sure how I stumbled on the route that gave me the option in the drop down for engrave

Quote:

---

Originally Posted by tom.jelly

No actually it looks like the attached, with the only choices being rough contour face or thread mill. I started by clicking on new 2.5 axis mill operation in the second down from the top tool bar. I'm still not sure how I stumbled on the route that gave me the option in the drop down for engrave

---

Ahh, I see the problem. You're inserting operations, not features. CAMWorks (Solidworks CAM) has three different tabs within Solidworks that you can work within. The feature tree, the operation tree and the tools tree. You're inserting an operation directly to the operation tree without there being a feature to define what you want to do. Try going to the CAMWorks Feature tree tab and inserting a new FEATURE instead of OPERATION.

https://i.ibb.co/w6FV36k/CW2.png

The flow in CWx or SWxC should always be from left to right starting with the Solidworks feature tree, then CWx/SWx Feature Tree, then CWx/SWxC Operation Tree. The tools tree is kind of optional. Does that make sense?

Thanks, that is the fix!
t