[HannesN]

Hi,

My 2. question in 2 days. Hope you do not mind!

I am looking for a solution to easily and hazzle-free insert tabs/bridges to simple 2.5D parts. Lets say I wanna cut a simple square out of a sheet of MDF . How to keep the square in place while routing - with thin tabs, right? Is there any built in tabbing in solidcam as for Vectrics Cut2D or a straight forward workaround/hack to achieve the same?

Also being challenging here: These tabs should be aligned to the 'bottom' of the part and only be a fraction as high as the part itself - not to just say very thin.

I'd very much appreciate your kind help on this one! Looking forward to hear from you.

Best, Hanns

[metalworkz]

Hello Hanns,
I don't know about Solidcam but for Cut2D there is a tab option on profile toolpaths in the newer version. Adding tabs to the toolpath in Cut2D is very easy and pretty much drag and drop on the vectors.
There are some other ways to achieve keeping the part in the blank and the 'onion skin' or 'foiled' option has worked for me on various materials. When cutting the profile of you part simply set your cutting depth about .015" short of the actual material thickness for wood(I have used this with redwood and poplar but not MDF yet) For materials like aluminum you can do the same thing only much less material can be left to hold the parts, and probably .002" to .005" should be enough to foil the part in the blank. It is fairly easy to break most of the foiled material from the part and usually not hard to finish cleaning up the edges.
There is another option that works very well with sheetmetal fabrication and I have seen it work well with aluminum and that is the machining version of a micro-joint on the corners of the part. For example on a square part make your profile vectors so that there are 4 separate toolpaths that cut within about .020" of each other at all four corners at the ends of the cutting toolpath. That small .020" to .030" wire tab will normally hold the part very well in the blank and it is easily cleaned up as there is only a small protrusion at each corner after breaking out of the blank.
You might be advised to try these methods on a small scrap part to see which one will work for you and you might have to modify the last option if needed to increase the wire joints or make them smaller.
I hope something here helps you out!

[HannesN]

Hi Wes,

Thanks for your reply! I tested the onion skinnig on MDF and my results were unfortunately pretty poor. The material is just to brittle and not really made for this nice workaround.

I guess the tabs are just a very straight forward and 'headache of post processing the part' - free tool and I am quite surprised it's so not obvious to do in SC.

Thanks again, Best, Hanns

[metalworkz]

Hello again Hanns,
Did you look at the other option I mentioned at the end of my post? It does not involve creating tabs(so to speak) but it does leave the material tabbed at the corners. You can simply increase or decrease the tab width by how long you make the vectors for each side and end up with probably a good method to hold the part without doing any special work for bridges of tabs in programming. Odd shaped parts may be a bit more work but if you have an offsetting tool in your drawing software it might not be too bad. Good luck with your project!

[HannesN]

Hi Wes,

Now I got it. Yeah that sounds like a clever idea. So not doing 'horizontal', but instead 'vertical', right? I will look whether this is more feasible for me to accomplish in SC/SW than the thin horizontal ones. I'd almost say it is. I'll come back when I have results.

Still if someone out there is having a worklflow to do this I would very much appreciate to hear about it.

Thanks, best, Hanns

[Brakeman Bob]

Hans,

The way I deal with tabs in SolidCAM is to create surfaces in the part called CAM in the assembly that SolidCAM creates when you start a *.PRT file.

This is more SW than SC, but here's how I do it. I create sketches using a surface of the DesignPart as the sketch plane. Then extrude the sketch by however thick you want your tab. In Aluminium I use 0.15mm

Bob

[HannesN]

Hi Bob,

Thanks for your reply; was seeing your post just now after some more hazzle with tabs.

I actually do the tabs as you proposed; so SW-wise no real problem.

Just to recall: I am looking to keep simple flat pieces in place while milling profile operations on a 2.5d job.

So what I want to have is either a.) a 'vertical' tab - the tool path of the profile operation describing the perimeter of the part simply does not mill where the tabs are - or b.) a 'horizontal standard' tab as in packages like Cut2D.

For now I can't think of a simple and evident workflow for achieving one of these options - both approaches involve massive 'path-picking work' and multiple passes and for that are quite a pain when 'rapid' prototyping.

I'd very much appreciate your sharing of ideas and approaches. Looking forward to hear from you.

Thanks a lot, Best, Hanns

[mykrowyre]

Hans, did you ever find a good way to do tabs in solidcam? I've been researching this for a few weeks now, and like you, I have not found a straight forward way to do this. Yes, I can add the tabs when creating the part, but as you said this means doing lots of path picking in solidworks.

Would be interested to hear which method you finally settled on.

Thanks
tom

[HannesN]

No method I settled to. Just coming back to this issue now. It's a pain and I can hardly believe it's supposed to be done the way described in the thread. Would be happy to hear back from you and anyone who has a good idea. Best, Hannes

[tjfdownsouth]

If you are milling MDF or UHMW then i usually stop my profile cut short of going all the way through the last path like 0.02. This leaves a paper thin piece left to hold the part in place which can easily be removed with a utility knife. In wood this doesn't work because it splits with the grain so i have to do the SW method.

Tim

[HannesN]

Hi Tim, Yeah sure that's how I work around it as well. Nevertheless that's not to satisfying. I'll start a new thread being more precise of what I think of from beginning. Thanks, Hannes

[guru_florida]

Reviving an old thread here but, after you create the tabs in the CAM part....how do you machine around them using simple Profile operation? If I am selecting/creating a profile around the actual part, then there is no way to subtract out the tabs. There is also no check surfaces anymore.

Hans,

The way I deal with tabs in SolidCAM is to create surfaces in the part called CAM in the assembly that SolidCAM creates when you start a *.PRT file.

This is more SW than SC, but here's how I do it. I create sketches using a surface of the DesignPart as the sketch plane. Then extrude the sketch by however thick you want your tab. In Aluminium I use 0.15mm

Bob

[jaras]

I would also like to find an answer to this, no one worked it out? Additional plugins or something else?

[guru_florida]

I did figure it out. It's basically a Solidworks solution. I'll start off with the simplest method, then I will describe how you can do it while working in Solidcam. So....

Method 1:
Simply make tabs a feature of the part. So create a new sketch, select the bottom of the part as the new sketch plane. Now draw some rectangles that attach to the part that will become the tabs. Now, because the tool is round (duh) your tabs are going to be more like an hourglass shape after being cut. You could model them properly with the right tool diameter but why bother, just give the tab the proper width to take into account the "gouge" that will occur. So for a 0.25" dia tool, and you want a tab that is 0.15" wide, go with 0.35" tab width. Make the tab extend out of the part by 0.35" but really the extension length is inconsequential. I use a 15mil tab thickness (depth), this let's me punch the part out after by hand but still provides lots of stability during those final cuts.

You can now create two part configurations, the default one has the tabs suppressed while the other config has the tabs active. In Solidcam you can specify the target config you will be cutting.

Now in solidcam, define your typical profile toolpath as you normaly do, but only go down to the top of the tab. Now to cut the tabs create another profile path, but this time instead of selecting the whole part profile, you will create multiple open paths/chains that run in-between the tabs. You will have to select each path segment in between the tabs, and will have to switch between selecting line segments and points. For example, when you are approaching a tab, you will have to switch to point selection and select the intersection point where the tab meets the part. Then add/OK this path segment and start the next at the point opposite the tab. So really the tabs are just acting to create those "points", we dont actually create paths/profiles with the tab geometry itself.

Method 2:
Basically, you do exactly the same as above but instead of adding the tab sketch to the part, you add it to the SolidCAM assembly document. It get's merged with the part, but doesnt affect the original Solidworks part. Make sure to specify both the part and the tabs as the TARGET during your solidcam definition otherwise you will not be able to select points in the geometry.

By adding Profile operation templates for the "profile down to the tab" and "profile the tab" I can now handle the creating of tabs pretty easily/quickly and I like having the power of solidworks to define the tabs.

Going with tabs has been much better. No more nicks when the part releases, nor any hanging metal leaf-like left-overs, and definitely much safer! I can punch the part out with my fingers and hand file the tab stubs easily.

I do suggest doing method 1 first. You might be tempted to jump to modifying the SolidCam assembly, but that has some challenges too and I found until I had the first method down, I couldnt figure out the intricacies of the second method.

Good luck!

[jaras]

Sweet! I'll try out your method one to night. If I get this working I'll vote this answer as number one solidcam tip ever :-)

[jaras]

It did work :banana: that is so sweet! Many thanks to you guru_florida. What I did is that I used Solidworks and added two open chains with the point to point option. As you said that is the easiest to figure out. Now when I got it going it should be an easy task from solidcam by just adding points instead of drawing the whole tab.


-

[guru_florida]

Glad to hear! Your pics look right. When you switch to doing it in SolidCAM it is the same process, except you are adding it to the SolidCAM assembly that is created when you first create the SolidCAM part. The benefit is that the original solidworks part is not modified, and the effort is the same once you know it - as I said, just remember to select both the part body and tabs body in the TARGET selection.

I had some difficulty with doing it on the solidworks side. Using a new configuration worked great, but then in solidcam it would often forget the "config name" and switch back to the default config which popped up the "resync" dialog a lot. Solidcam is sooo buggy. So it worked better if I did it in solidcam. I just mentioned the solidworks way first because it is easier to figure out the first time.

It did work :banana: that is so sweet! Many thanks to you guru_florida. What I did is that I used Solidworks and added two open chains with the point to point option. As you said that is the easiest to figure out. Now when I got it going it should be an easy task from solidcam by just adding points instead of drawing the whole tab.


-

[guru_florida]

I was in solidcam today, so I thought I would post some of my pics. First shot is of the feature tree, notice I am not in the solidcam tab, but the Feature Manager one. The SolidCAM assembly contains two parts, the "CAM" part, and the "DesignModel" one. The DesignModel one is my actual part I want to cut. The CAM one is essentially an empty part that I can add stuff too, that can also reference sketches/features in the DesignModel.

So in the CAM part, I:
1. edit it part in place
2. add a new sketch
3. sketch the tabs
4. close sketch and extrude them
5. close the part

My feature tree now looks like in the pic, notice the added feature "MyExtrudedTabs".

Now back in the SolidCam tab, I right click Target under "CAM-Part", click Define, then using that option select both my part and tabs as the design model. Then OK.

Now in my operation I create the toolpath chains like in the second pic, using the point-to-point tool, and the whole line segment tool.

Voila!

[jaras]

Hi, I followed your instruction and created tabs from solidcam and that works as well. Great.
I tried a different approach and just added sketch points instead of creating full tabs but that was not successful.

[Aussie_CNC]

Hi all,

In SolidCAM 2012 SP2 onwards there is a new operation dedicated to tabs. It is one of the toolbox cycles - "Four nubs cycle", it hasn't been named well (and they are termed "bridges" in the technology page) but you can simply input the number of tabs you want (you are not limited to 4 as the operation name suggests).

Hope this helps!