TM CAD - Upgrade or Delete?

[BrayD]

I'm a fairly advanced user of CAD systems. I've used Solidworks (and recently Inventor) for the last 15 years of my professional career and I hold a commercial license of Fusion360 / Bendtech SE for the stuff I do at home. I bought an old 5x10 Torchmate table running TM2 and I just got it running last week. It came with TM CAD version 5. I want to upgrade the computer that it came with (i.e. get the Torchmate stuff onto my modern shop computer), but Torchmate is telling me version 5 won't run on my Windows 10 Pro machine.

I can upgrade to the latest TM CAD (for ~$1k) or abandon it entirely and use my other systems to generate cut paths. I'm trying to determine the value of TM CAD. Should I keep it or save my pennies? Read on for more detail.

Are all DXF's Created Equal?

Even with my experience in CAD, I rarely had to work with DXF's. I've also found that all DXF's may not be created equal, as some shops struggled to use those that I created from Fusion or Bendtech. One example I can think of is when I sent a DXF of a flat pattern to a shop, apparently it still had bend lines on it - they cut the bend lines. I could certainly brush up on my DXF creation / editing skills in these other softwares, but it's kind of nice to do all of that work in TM CAD then send it directly to the driver software. Do you guys run into these issues when generating DXF's in software other than TM CAD when sending it to the driver software? Can you specify cut order/direction in Fusion? I still don't understand how that info gets stored in a dxf, but when I import a TM CAD dxf into TM2, it generates the g code on import and it all just works.

Image Tracing

This is also something that I rarely had to do for my professional career, however I can see it becoming a large part of my workflow with the torch table. I have Inkscape, but being new to all of this I'm a very light user. I understand that the recent TM CAD has a pretty solid tracing tool. Does anyone prefer it over Inkscape?

Compatibility

I don't really know how to explain this, but TM CAD coupled with TM driver software seems like a match made in heaven. I don't want to spend money and commit to their proprietary software just because it gives me the warm and fuzzies though. If I can achieve the same thing in similar time using software that I already have, that's probably the route I should go. I feel like I'm racking up a good deal of redundant software at this point: Fusion, Bendtech, Inkscape, TM CAD.

What does TM CAD have that these other softwares lack?

[weldguy]

I am not familiar with TM CAD myself so I cannot answer your closing question. I do have Fusion experience and I read you also have Fusion and I expect it would do everything you would need aside from simple image tracing. If I were in your shoes I would run with Fusion 360, save $1K and in my experience it outputs really good DXF's. Would be interesting to hear from a TM CAD user.

[adbuch]

You can download a free trial version of TMCad 9 at the link below. It will run on your windows 10 computer, and is fully functional except that it will only save in .edu format. Nevertheless, it will give you an opportunity to see how it differs from your older version.

https://torchmate.com/training-header/t ... -downloads

David

[adbuch]

Are all DXF's Created Equal?

Even with my experience in CAD, I rarely had to work with DXF's. I've also found that all DXF's may not be created equal, as some shops struggled to use those that I created from Fusion or Bendtech. One example I can think of is when I sent a DXF of a flat pattern to a shop, apparently it still had bend lines on it - they cut the bend lines. I could certainly brush up on my DXF creation / editing skills in these other softwares, but it's kind of nice to do all of that work in TM CAD then send it directly to the driver software. Do you guys run into these issues when generating DXF's in software other than TM CAD when sending it to the driver software? Can you specify cut order/direction in Fusion? I still don't understand how that info gets stored in a dxf, but when I import a TM CAD dxf into TM2, it generates the g code on import and it all just works.

No - not all cad programs save dxf files in exactly the same format. But not all cad programs offer the option to export as svg or other vector formats.
Yes - you can specify the cut order with Fusion 360. The cut order, etc. does not get stored in a dxf. It does get stored in the .f3d format.

David

[adbuch]

Image Tracing

This is also something that I rarely had to do for my professional career, however I can see it becoming a large part of my workflow with the torch table. I have Inkscape, but being new to all of this I'm a very light user. I understand that the recent TM CAD has a pretty solid tracing tool. Does anyone prefer it over Inkscape?

TMCad will do image tracing. I do have a TMCad 9 (paid perpetual license) installed on a Windows 10 computer and am familiar with may of it's features, but I prefer Inkscape for auto tracing. I use either Inkscape or CorelDraw for manual tracing, depending on the particular image I am tracing.

David

[adbuch]

Compatibility

I don't really know how to explain this, but TM CAD coupled with TM driver software seems like a match made in heaven. I don't want to spend money and commit to their proprietary software just because it gives me the warm and fuzzies though. If I can achieve the same thing in similar time using software that I already have, that's probably the route I should go. I feel like I'm racking up a good deal of redundant software at this point: Fusion, Bendtech, Inkscape, TM CAD.

You don't necessarily need TMCad for generating cut paths and post processing. SheetCam will perform these functions from an imported dxf or svg file. There are several Torchmate post processors available in SheetCam and one of them should work fine for you.

David

[adbuch]

What does TM CAD have that these other softwares lack?

TKCad does have a Polyarc tool that some of the other lack. That is the reason I purchased a TM license. It will also let you specify the dxf export format.
David

[BrayD]

Great info. Thank you!

I did some playing around tonight and opened the door to Fusion CAM. I've never explored this environment before. At first glance, it seems more than powerful enough to do what I want to do, it's just going to take some time to learn it. I did, however, use it to successfully generate a cut path and G code for this week's DXF download "VW Bus". It appears like it will cut properly in the TM2 driver software, but I'm hesitant as Fusion only has post for TM3 rather than TM2. More research/exploration is required before I'll be comfortable running my table with the G code it generates.

Good to know you prefer Inkscape for tracing. That will motivate me to dive into that software and learn my way around it.

Thanks for highlighting the different DXF export types also. Much to learn. In the meantime, TM CAD 5 is still up and running on the old computer that came with my table. This isn't an urgent change, but if something happens to that computer I'll be left with a decision to make (that thought was the genesis of this thread).

[adbuch]

Great info. Thank you!

I did some playing around tonight and opened the door to Fusion CAM. I've never explored this environment before. At first glance, it seems more than powerful enough to do what I want to do, it's just going to take some time to learn it. I did, however, use it to successfully generate a cut path and G code for this week's DXF download "VW Bus". It appears like it will cut properly in the TM2 driver software, but I'm hesitant as Fusion only has post for TM3 rather than TM2. More research/exploration is required before I'll be comfortable running my table with the G code it generates.

Good to know you prefer Inkscape for tracing. That will motivate me to dive into that software and learn my way around it.

Thanks for highlighting the different DXF export types also. Much to learn. In the meantime, TM CAD 5 is still up and running on the old computer that came with my table. This isn't an urgent change, but if something happens to that computer I'll be left with a decision to make (that thought was the genesis of this thread).

Happy to help! It might be a good idea to back up your TMCad 5 program files so that if something happens to the old pc you can install it onto a similar functional pc. I happen to prefer AutoCad R14 for certain tasks - and it won't run on anything newer than Windows XP. So I've got installed on my original Gateway Windows 2000 pc along with a newer Windows xp pc out in the shop. I use it in conjunction with MasterCam 9 - which also only runs on the older Windows operating systems.

David

Sheetcam offers several Torchmate post processors, and there is a free version (limited file size - line length). You might consider taking a look at it as another option. You can draw your part in just about any cad program, save as dxf or svg, and import to SheetCam for tool path creation and post processing.

I personally think it is quicker to use several programs in combination - Inkscape/SheetCam, CorelDraw/SheetCam, etc. than to do the cam/post processing with Fusion 360. Also - Fusion 360 has been know to run slowly or hang up - particularly with larger files due to being cloud based and depending on their server for computations. SheetCam would not have that problem.

I personally don't need to use SheetCam, since I have a Plasmacam table and the Design Edge software does everything - draw, create cut paths, and post process.

[adbuch]

You might also consider using a sharpie pen holder attached to your torch and draw (instead of cut) for your testing. Let your table draw the part so you can see what it looks like instead of wasting metal. There is a discussion at the thread below.

David

viewtopic.php?p=236518&hilit=sharpie+pen+holder#p236518

[BrayD]

I've downloaded SheetCAM and I'm starting to lean into it. I think it'll be a great TM CAD replacement if necessary. During this whole process, I tried making a test dxf from Fusion that I could import into the other software to generate cut paths/G code. In doing so, I found that my version of TM CAD crashes when importing a Fusion dxf. All the more reason to move to SheetCAM as it opened and generated a cut path/G code without issue.

In an attempt to reconcile the differences between TMCAD and SheetCAM, I needed a simple DXF that would work with both of them. BendTech provided that solution. Simple 2" square with a 1" hole. Exported using the 'Plasma dxf Export' tool and it worked beautifully. Worth noting that I didn't have the option to select the dxf type though (line vs polyline vs polyarc).

My challenge now is modifying the post in SheetCAM to give me G code that my driver software will be happy with.

This is what I'm getting from TM CAD. The workflow is to import the dxf into TMCAD, generate the cut path, then export a dxf from that software (no option to export G code).

From the driver software, I 'import dxf' and select the TMCAD dxf file. It instantly prompts me to name and save a G code (.fgc) file, then it displays the cut path in the working window. I went ahead and 'ran' this while offline to ensure it followed the proper path. Resulting image including the TM G code is shown below.

Next up is SheetCAM. Simple workflow and it creates the G code in seconds. There are multiple Torchmate posts to choose from, however none of them are intuitively for my machine (TM2). I'm able to modify these posts and have no issue doing so, I just need to understand what's going on so I can modify accordingly. I started by changing the M03/05 commands to M50/51 for torch start/stop, as I know that's listed in the TM2 driver software. Cut path, post type, and resulting G code below.

SheetCAMpostEdited.png (30.82 KiB) Viewed 3524 times

SheetCAMpostEdited.png (30.82 KiB) Viewed 3524 times

Trying to run that G code in the TM driver software yields the following errors:

None of that is concerning to me at the moment. I can modify as necessary once I figure out what I'm doing.

Found a SheetCAM post labeled 'Torchmate THC' so I ran that. The result is no M code nor Z control. Very similar to the TMCAD G code. It actually runs in the driver software too. Could this be the one?

Posting this while I have internet access. Heading to the shop now to see how it controls the table.

[BrayD]

That'll work! I still don't understand how it knows when to turn the torch on, when to turn the torch off, when to raise the torch head between cuts, etc. All of that must be handled in the TM controller based on the motion G code. Pierce and cut height are set on the AVHC so I guess it's not too much of a stretch for me to connect the dots.

Either way, I'm officially freed from the TMCAD handcuffs.
.

cutinprogress.png (235.72 KiB) Viewed 3521 times

cutinprogress.png (235.72 KiB) Viewed 3521 times

part.png (206.89 KiB) Viewed 3521 times

part.png (206.89 KiB) Viewed 3521 times

.
My Inkscape skills are improving as well. My boy loves music so I traced and cut him a simple guitar yesterday. I think Inkscape/SheetCAM will be a solid solution going forward for the more artistic work. Fusion and BendTech are still options for design of mechanical parts. It's awesome having everything loaded right here on my laptop. Design in-house. Manufacture in-shop.

Please ignore the cut quality. Now that I can run the thing reliably I can start getting it dialed in.
.

guitar.png (196.58 KiB) Viewed 3521 times

guitar.png (196.58 KiB) Viewed 3521 times

[adbuch]

I still don't understand how it knows when to turn the torch on, when to turn the torch off, when to raise the torch head between cuts, etc. All of that must be handled in the TM controller based on the motion G code.

It looks like you are making great progress! Here is some explanation of the g-codes in the program you showed above.

David

gcode.jpg (78.83 KiB) Viewed 3511 times

gcode.jpg (78.83 KiB) Viewed 3511 times

[adbuch]

https://www.sherline.com/g-code/?srslti ... D2lrPS7Og2

[BrayD]

Ah yes, that all makes perfect sense to me. That's the post that I modified to specify the M50/M51 torch start/stop. When I ran that G code through the TM driver software it resulted in errors though.

When I selected the Torchmate THC post in SheetCAM, it gave me G code without any M code or Z heights. This program ran perfectly in the driver software and cut the physical parts. Still a mystery to me how it can control the torch and Z, but it must be handling that in the background through the TM controls.

This is the G code that ran properly on the table, produced by SheetCAM.

.

sheetcam TM THC G code.png (37.06 KiB) Viewed 3485 times

sheetcam TM THC G code.png (37.06 KiB) Viewed 3485 times

[jlasater]

I have a TorchMate 4400 with the AccuMove 2 controller and based on what others suggested, I just cycled through all 5 (or more) TorchMate post processors were available and in my case the VMD2 one worked perfectly. I didn't have to modify the postprocessor at all once I found the right one. The ones that didn't work would distort the cut shape dramatically. I ended up using QCAD and SheetCAM for work flow and it's all working great.